CamBam

Resources => Scripts and Plugins => Topic started by: pstemari on August 11, 2013, 21:44:33 pm



Title: V-Engrave Plugin
Post by: pstemari on August 11, 2013, 21:44:33 pm
I've finally got a working version of the v-engrave plugin available for download.

The code is up at http://code.google.com/p/v-engrave-plugin/ and you can download a compiled plugin at https://v-engrave-plugin.storage.googleapis.com/v-engrave-plugin-latest.zip

There's an issue with overshoot with smooth corners, most noticeable if you have a smooth corner opposite a sharp inside corner, so check your toolpaths with a cut viewer.


Title: Re: V-Engrave Plugin
Post by: atwooddon on August 11, 2013, 21:47:40 pm
Great, thanks for all your work.  There are many of us waiting to try out your code.  Will post results.

thanks again.

Don


Title: Re: V-Engrave Plugin
Post by: lloydsp on August 11, 2013, 22:03:00 pm
For those of us not running Linux, or who don't have git, can you zip up the repository for a WinBlows download?

Thanks for this.  We've been waiting with 'bated breath for your code examples!

Lloyd


Title: Re: V-Engrave Plugin
Post by: pstemari on August 12, 2013, 03:53:04 am
Done.

Note that there's a easy git install for Windows available at http://git-scm.com/download/win.

There's also an issue tracker at http://code.google.com/p/v-engrave-plugin/issues/list.  You may need to have a Google id to be able to post bug reports there. 


Title: Re: V-Engrave Plugin
Post by: pixelmaker on August 12, 2013, 12:24:03 pm
Thank you for this plugin.
I have already translated and extensively tested last night.
It looks very good, even with complicated contours are well.
The attached file is a challenge for any  v-carve software.
But it looks very good.


Title: Re: V-Engrave Plugin
Post by: blowlamp on August 12, 2013, 12:39:53 pm
A very nice addition to CamBam, thank you.

pixelmaker.

Did you forget to post the file, or did you mean the pictures you attached?


Martin.


Title: Re: V-Engrave Plugin
Post by: Bubba on August 12, 2013, 12:57:41 pm
Great. Thanks for the much needed addition to CamBam.

Here I have an issue with it working for me.

Downloaded the file, unzipped to its own folder because 7zip will not unzip it to the *.* CamBam/ Plugins directory. Moved the VEngrave_Plugin.dll to CamBam/plugins directory. It is recognized by CB but I can not get it to work.. Any suggestions


Title: Re: V-Engrave Plugin
Post by: lloydsp on August 12, 2013, 13:02:44 pm
Heh!  You just clicked on the plugins/about V-engrave!

Go to "machining", and you'll see a new MOp type!

Lloyd


Title: Re: V-Engrave Plugin
Post by: Bubba on August 12, 2013, 13:10:24 pm
Thanks Lloyd.
Because all (most) of my plugins reside in the plugin directory (highmap, ArcText, etc) I failed to look for it anywhere else.  Thanks for the tip.. ;) ;D


Title: Re: V-Engrave Plugin
Post by: pixelmaker on August 12, 2013, 14:10:11 pm
Quote
Because all (most) of my plugins reside in the plugin directory

Not the Thread Milling Plugin  ;D

ralf


Title: Re: V-Engrave Plugin
Post by: dh42 on August 12, 2013, 16:34:43 pm
Hello,

Very nice job, thanks  ;D

I get some little bugs:

The MOP's icon switch from red V tool to a green arc icon when I enter value in the MOP.

The VEngrave MOP return an error message if I try to copy it.

++
David



Title: Re: V-Engrave Plugin
Post by: lloydsp on August 12, 2013, 17:33:37 pm
The VEngrave MOP return an error message if I try to copy it.

----
Maybe not a bug in V-engrave, but merely that CB does not recognize it as a valid MOp, because it is not one of its native types?

Lloyd


Title: Re: V-Engrave Plugin
Post by: dh42 on August 12, 2013, 18:27:57 pm
Hello,

Not sure, the lathe MOP is also a plugin, and copy/paste and copy/paste format works.

EDIT: another thing, the value of Path step size is not saved in the .cb file and must be changed each time the file is opened, but maybe it's not possible without changing the .cb file format ?

++
David


Title: Re: V-Engrave Plugin
Post by: BR52 on August 12, 2013, 19:46:50 pm
Hello pstemari,
To change the MOP and save the file.
And copying a MOP.
You need Add Reference:
"System.Runtime.Serialization"

Please see attached photos.

      Armando


Title: Re: V-Engrave Plugin
Post by: Bubba on August 12, 2013, 19:51:46 pm
I like the HELL out of the new V-carve MOP! Thanks!.

 Bubs or no bugs.. ;D ;) :D


Title: Re: V-Engrave Plugin
Post by: pstemari on August 13, 2013, 06:18:49 am
> You need Add Reference: "System.Runtime.Serialization"

That's already in there.  Without it you can't save at all.

I'm not sure what the cut & paste issue is.  If the save issue above is just a single attribute I probably just missed setting the flag.


Title: Re: V-Engrave Plugin
Post by: pstemari on August 13, 2013, 07:17:02 am
Ok, issue 9 is fixed. 

Build b0002 has been uploaded to http://v-engrave-plugin.storage.googleapis.com/v-engrave-plugin-latest.zip


Title: Re: V-Engrave Plugin
Post by: 10bulls on August 13, 2013, 09:15:00 am
Wow! Thank you for your brilliant work on this Paul.

I haven't check this, but the copy & paste issues may be due to not having a...
[Serializable]
attribute on your MOPVEngrave class.
Any serialized custom classes used within the MOPVEngrave also need to be marked as serializable.

I hope this helps and thank you again!



Title: Re: V-Engrave Plugin
Post by: BR52 on August 13, 2013, 13:20:31 pm
The correct address is:
https://code.google.com/p/v-engrave-plugin/wiki/Downloads

Has no function change the properties of the MOP  ???
Example diameter and angle of the tool is the same old value.
Note the comment from David and Andy.

     Armando


Title: Re: V-Engrave Plugin
Post by: dh42 on August 13, 2013, 14:49:47 pm
Ok, issue 9 is fixed.  

Build b0002 has been uploaded to http://v-engrave-plugin.storage.googleapis.com/v-engrave-plugin-latest.zip

Hello,

no change for me (and it was already a b0002 in the download, but say b0001 in the "about"), the value of Path step size is not saved.

++
David

EDIT: Ok,  :-[ I download the wrong file (v-engrave-plugin-latest.zip) the right link is v-engrave-plugin-b0002.zip ...  and the problem is solved, but it show always "b0001" in the "about" (and also in the Windows properties/version panel)


Title: Re: V-Engrave Plugin
Post by: BR52 on August 14, 2013, 12:05:04 pm
Hi David,
I just want some help finding BUGs.
You made ​​a video here:
http://code.google.com/p/v-engrave-plugin/issues/detail?id=12

        Make a video showing this BUG:
In the properties window in MOP VEngrave1 with the right mouse tries to copy.

pstemari, the file "v-engrave-plugin-src-b0003.zip" is empty  ???

      Armando


Title: Re: V-Engrave Plugin
Post by: dh42 on August 14, 2013, 13:41:17 pm
Hello Armando,

No problem for me to download the b0003 ; I add it in attachment

It solves the problem with MOP copy.

++
David


Title: Re: V-Engrave Plugin
Post by: BR52 on August 14, 2013, 14:33:00 pm
David thank you very much,
OK worked great but the file "v-engrave-plugin-src-b0003.zip" is empty.

    Armando


Title: Re: V-Engrave Plugin
Post by: dh42 on August 14, 2013, 15:02:55 pm
Quote
OK worked great but the file "v-engrave-plugin-src-b0003.zip" is empty.

Yes, same for me, I had not seen that it was the source file that you want  :-[

++
David


Title: Re: V-Engrave Plugin
Post by: pstemari on August 14, 2013, 17:37:48 pm
Sorry about that.  Should be good now.


Title: Re: V-Engrave Plugin
Post by: pstemari on August 19, 2013, 07:13:19 am
I just uploaded b0004.  This includes fixes for issues:

3 (https://code.google.com/p/v-engrave-plugin/issues/detail?id=3)Overshoot on smooth corners
4 (https://code.google.com/p/v-engrave-plugin/issues/detail?id=4)Max depth/cutter diameter is not implemented
6 (https://code.google.com/p/v-engrave-plugin/issues/detail?id=6)Default step size is too small for mm-based projects
7 (https://code.google.com/p/v-engrave-plugin/issues/detail?id=7)Wrong MOP icon
8 (https://code.google.com/p/v-engrave-plugin/issues/detail?id=8)Can't copy a V-engrave MOP
9 (https://code.google.com/p/v-engrave-plugin/issues/detail?id=9)V-engrave MOP spécific datas are not saved in .cb file
12 (https://code.google.com/p/v-engrave-plugin/issues/detail?id=12)ToolPath display bug if Stock surface <> 0
16 (https://code.google.com/p/v-engrave-plugin/issues/detail?id=16)Infinite loop/bad toolpath


Title: Re: V-Engrave Plugin
Post by: Bubba on August 19, 2013, 18:49:17 pm
Is only the V 90 deg cutter used with this plugin? Is any thought of adding a V60 deg cutter as well. Smaller test would look better cut with V60. Thanks.


Title: Re: V-Engrave Plugin
Post by: lloydsp on August 19, 2013, 19:13:08 pm
Huh?  Just set your own angle!  90-degrees is the default setting.  You can change it.

Lloyd


Title: Re: V-Engrave Plugin
Post by: pstemari on September 16, 2013, 05:45:27 am
I just uploaded b0005.  Nothing major, some fixes for the z-position at the beginning and end of each cut.  The behavior with rapids should be better.   See Issue 18 (https://code.google.com/p/v-engrave-plugin/issues/detail?id=18) for details.


Title: Re: V-Engrave Plugin
Post by: BR52 on September 16, 2013, 18:42:32 pm
Hi

The problem is in the "post processor", I created a "post processor" see attached.
Second, I create in library tool, a tool see picture attached.

     Armando


Title: Re: V-Engrave Plugin
Post by: pstemari on September 18, 2013, 00:04:01 am
CamBam doesn't copy that field from the tool library to the MOP with the diameter, etc.  That's why the V-Engrave mop has a V Angle setting, as well as a tip diameter, which doesn't exist in the tool library at all. Getting the tip diameter entered correctly is quite important for actual engraving.

I might be able to find the item i the tool library and try to duplicate the base logic for when to use tool library values instead of a local value, but that gets rather complicated.


Title: Re: V-Engrave Plugin
Post by: Jeff_Birt on September 18, 2013, 00:27:32 am
By 'tip diameter' do you men the tip flat, i.e. the width of the flat at the tip of the bit? By saying 'diameter' you are likely to cause confusion as there re tapered ball end mills that do have a tip diameter, i.e. the diameter of the ball end.


Title: Re: V-Engrave Plugin
Post by: lloydsp on September 18, 2013, 00:29:57 am
But, Jeff, the discussion is "V-Engrave Plugin".  I haven't yet mastered Vee engraving with ball-end mills! <G>

Lloyd


Title: Re: V-Engrave Plugin
Post by: BR52 on September 18, 2013, 02:41:08 am
It is unfortunate not to have seen the two files that I attached.
Your file "TestVEngrave6.cb" is wrong.

     Armando


Title: Re: V-Engrave Plugin
Post by: Jeff_Birt on September 18, 2013, 03:50:37 am
But, Jeff, the discussion is "V-Engrave Plugin".  I haven't yet mastered Vee engraving with ball-end mills! <G>

Lloyd


That is my point Lloyd. Using the term 'diameter' when talking about the tip flat is confusing.


Title: Re: V-Engrave Plugin
Post by: dwc on September 18, 2013, 07:47:58 am
By 'tip diameter' do you men the tip flat, i.e. the width of the flat at the tip of the bit? By saying 'diameter' you are likely to cause confusion as there re tapered ball end mills that do have a tip diameter, i.e. the diameter of the ball end.

The engraving bits I see for sale with different shoulder angles all have a diameter at the point, not a flat.
A flat seems to be counter intuitive for engraving to me and less useful.
Where to they come from the engravers with a flat?
Don


Title: Re: V-Engrave Plugin
Post by: lloydsp on September 18, 2013, 12:02:23 pm
Jeff,
That's why we refer to ball-end mills by 'tip radius', and the flats on v-engravers as 'tip diameter'.  'least... that's the way I was always taught to differentiate them.

Don,
"A flat seems to be counter intuitive for engraving to me and less useful.
Where to they come from the engravers with a flat?"

Most two-flute types have a 'drill bit-like' face, not unlike that of twist drill or an end mill.  It's not truly a flat -- It's really two 'wings' that cause a circular flat-milled surface when touched to the work.  The face-ends of the two flutes are beveled and sharpened.  Don't ask ME how they work a flute that small!  I'm still trying to figure out 10-mil diameter carbide twist drills! <G>


All my good carbide v-mills are like that.  I have not a single one with a radiused tip.  You can get the carbide Vees all the way down to tip diameters of 2-mils.  The smaller they are, the easier they are to break, of course.  I won't even handle mine anywhere but on a rubber work pad.  Even a 2" drop to a metal surface might chip that little point.

Oh... for reasons cited earlier... don't buy the cheap off-shore cutters.  I get the best I can muster when I'm working with diameters that small.  A couple of mils runout on a cutter 2 mils in diameter is 100%!


LLoyd



Title: Re: V-Engrave Plugin
Post by: pstemari on September 18, 2013, 18:12:49 pm
Finally got out to the shop to make some chips.  The engraving (using one of Jeff's fabulous 2-flute carbide cutters), came out beautifully.  Still a little tripoli compound on there.  That stuff is hard to get off!


Title: Re: V-Engrave Plugin
Post by: pstemari on September 19, 2013, 06:54:02 am
Quote
Your file "TestVEngrave6.cb" is wrong.

What's wrong with the file, Armando?  The dot on the exclamation point wasn't cut in the previous build, but the current one fixes that issue.

I looked at the screenshot you posted earlier, but as I said, the plugin doesn't current try to get the v-angle from the tool library.



Title: Re: V-Engrave Plugin
Post by: BR52 on September 19, 2013, 13:04:49 pm
On "Mach3CVEngrave.cbpp" there are two macro of command.
The first command "TOOL/CHAMFER" activates the library CutViewer.
In the second command "TOOL/CHAMFER" puts the tool parameters.
The parameters are:
        TOOL/CHAMFER,{$tool.diameter},{$tool.veeangle},{$tool.length}

On CamBam you have to create a tool !
The tool V is a cone, the cone base is the diameter of the tool.
The cone base up to the tip and over the tool shank you have the total length.
You add a profile VCutter.
And finally add a command of macro "Vee Angle".

    Armando


Title: Re: V-Engrave Plugin
Post by: pstemari on September 20, 2013, 17:13:31 pm
Ok, I'm still confused.

The post-processor you posted adds comments to the g-code that CutViewer will use to get the tool geometry for its simulation.  That doesn't have any effect on the tool path or what your machine tool will do.  Mostly it saves you from having to re-entry the tool information into CutViewer.

Unfortunately CutViewer's notion of the tool geometry is more suited to chamfer mills than engraving cutters.  It uses the chamfer angle and the height of the chamfered part of the mill.  That length is 1/2*(tool dia-tip dia) * tan(90 deg - 1/2*v-angle).  AFAIK you can't readily do that math in the post-processor macros, but I've never played with the post-processors very much.

At any rate, none of that has any impact on the MOP or the toolpath.  Is there some problems with the MOP that I should fix or a feature you'd like to have?


Title: Re: V-Engrave Plugin
Post by: dh42 on October 12, 2013, 22:36:36 pm
Hello,

I'm writing a little doc about your plugin for French forums, and I just find a little bug maybe linked with the old issue #7

When we disable a V_carve MOP (by menu or space bar), instead of a gray icon, we get an green arc icon.

++
David

Edit: the link to the French doc.
http://www.atelier-des-fougeres.fr/Cambam/Aide/cam/Plugin_VEngrave.htm


Title: Re: V-Engrave Plugin
Post by: pstemari on October 19, 2013, 02:24:28 am
Well, that's weird.  I'm guessing I need a gray version of the icon and an appropriately magic name.


Title: Re: V-Engrave Plugin
Post by: jm82792 on November 12, 2013, 18:37:22 pm
I just bought CamBam since my 40 uses were up and I like it.
I'm getting this error with stock setting with text and random bits of geometry.


Title: Re: V-Engrave Plugin
Post by: jm82792 on November 12, 2013, 19:06:14 pm
I got it!
I guess my version of CamBam was 9.0 and not 9.8.


Title: Re: V-Engrave Plugin
Post by: lloydsp on December 31, 2013, 01:03:53 am
As I'm learning plugins and C#, I'm experimenting by trying to make every plugin source I could find re-build under VS2010.  And so far, good successes!

If the plugin is one that is already in my active plugins, I always test it before I re-build, save the old .dll, and only replace it with mine once the old is safely tucked away.

So, I tested VEngrave, and it worked, just as I would have expected.  I just did a small square.

Then I tested my re-built .dll, and it worked, too.  So I tried a circle, and mine failed!  So I restored the old .dll, rebooted CamBam, and the original VEngrave.dll I downloaded from here failed also!

Please, someone, give it a try with a plain circle, and nothing else special.

Hmmm!

Lloyd




Title: Re: V-Engrave Plugin
Post by: Bubba on December 31, 2013, 12:28:09 pm
As you wish.. ;D


Title: Re: V-Engrave Plugin
Post by: blowlamp on December 31, 2013, 13:29:16 pm
Lloyd.
My other V-carving software won't do a perfect circle either. Probably classed as a 'special case' because it would require a straight plunge with no horizontal movement needed.

Bubba.
By the looks of the V-engrave icon you're getting in the machining pane, I think you're using an out of date version.


Martin.


Title: Re: V-Engrave Plugin
Post by: pixelmaker on December 31, 2013, 14:04:05 pm
Martin,
I think the v-engrave plug needs a short horizontal path.
If you translate a circle in one axis about 2/100mm the plugin works

ralf


Title: Re: V-Engrave Plugin
Post by: Bubba on December 31, 2013, 14:11:20 pm
Lloyd.
My other V-carving software won't do a perfect circle either. Probably classed as a 'special case' because it would require a straight plunge with no horizontal movement needed.

Bubba.
By the looks of the V-engrave icon you're getting in the machining pane, I think you're using an out of date version.


Martin.

I thought it was the newest. Where is the latest version I can download from? Thanks.


Title: Re: V-Engrave Plugin
Post by: pixelmaker on December 31, 2013, 15:22:24 pm
The latest is the b0005
http://code.google.com/p/v-engrave-plugin/wiki/Downloads

ralf


Title: Re: V-Engrave Plugin
Post by: dh42 on December 31, 2013, 17:41:57 pm
Hello,

Same error for me with B0005

if circle -> error
same circle converted to polyline -> error

I just change Y diameter to 99% (X stay 100%) with the scale tool, and the error disappears.

@Lloyd: This plugin is translatable, did you test if it stay translatable after your re compilation ?

++
David


Title: Re: V-Engrave Plugin
Post by: lloydsp on December 31, 2013, 17:53:28 pm
I did, and it does not, so it must be a compiler setting, or an environment setting.

Lloyd


Title: Re: V-Engrave Plugin
Post by: Bubba on December 31, 2013, 21:36:08 pm
The latest is the b0005
http://code.google.com/p/v-engrave-plugin/wiki/Downloads

ralf

Thanks Ralf.


Title: Re: V-Engrave Plugin
Post by: dataway on January 10, 2014, 17:19:57 pm
Just wanted to say thank you for all your hard work on this new MOP it works great...

John


Title: Re: V-Engrave Plugin
Post by: lloydsp on January 10, 2014, 18:26:00 pm
Regarding this:

@Lloyd: This plugin is translatable, did you test if it stay translatable after your re compilation ?

--------------------

I tested the original Vengraveb004, and cannot see any translatable characteristics to it.

What did you find translatable?  Knowing what to look for, I might find it, if I knew where to find it.

Thanks,
LLoyd


Title: Re: V-Engrave Plugin
Post by: pixelmaker on January 10, 2014, 19:52:30 pm
Lloyd,

Quote
I tested the original Vengraveb004, and cannot see any translatable characteristics to it.
There are some special values in the vengrave b0004. "Max. Corner Angle, Tool TIP Diameter, Tool V-Angle.
This values and the info in the help window are translateable. The other values are the 'cambam values'

ralf


Title: Re: V-Engrave Plugin
Post by: lloydsp on January 10, 2014, 20:28:24 pm
Ok... those messages only appear in the log pane, correct?

I'm thinking maybe the logger automatically does translations.  I'll have to check that.

Lloyd


Title: Re: V-Engrave Plugin
Post by: pixelmaker on January 10, 2014, 23:46:34 pm
The values in the properties plane and the info text in the help field at the bottom.

These names and descriptions / info texts appear after first start the plugin in the translation plugin.
There, in the third Column the translation entered.
The two front columns the English names and texts appear only when a new feature for the first time is called. If I install a plugin and do not start it on, then names and texts do not appear in the translation list.

Screenshot 1 • The Properties window, fully translated. At the bottom is the Help field with the info texts.
Screenshot 2 • Andy's translation plugin with the translations for the plugin.

ralf


Title: Re: V-Engrave Plugin
Post by: lloydsp on January 11, 2014, 11:59:09 am
Yes, I know how all that works.  In fact, I have a demo plugin about to publish here that explains all that stuff about the translation files, how to invoke the translations, etc.

My point was, I can find absolutely nothing in the V-engrave plugin that does any translation calls directly.  Therefore, I must assume that some CB UI calls do them automatically.  I just haven't yet figured out which ones do the calls, and which ones do not.

I'll be publishing my translations source stuff as soon as I get one last 'feature' figured out.

LLoyd


Title: Re: V-Engrave Plugin
Post by: dh42 on January 11, 2014, 15:43:05 pm
Hello,

I have spent some hours, but no progress on translation ...

I explored the various compiler settings, but not change.

I also manually edited the translation file (translate_fr) to add text to the plugin, but they are not taken into account when the plugin run ..

I think we need help from Andy if we want to keep our hair  ;D

I have also not found how to add a sub menu (Edit / Transform / ...)

I will publish the new revision of the "NumMove" plugin earlier.

++
David


Title: Re: V-Engrave Plugin
Post by: lloydsp on January 12, 2014, 00:31:19 am
David,

I am CERTAIN, that the way I am doing it is not the way Andy implements it, but I have conquered it for limited applications like small plugins.

Find a new thread here in Scripts and plugins, giving a working example and source.

Lloyd


Title: Re: V-Engrave Plugin
Post by: macbob on February 04, 2014, 04:33:49 am
Er, OK, from the department of things that should never be repeated, I bring you - V-engrave with a paintbrush!

I rubberbanded a Pentel paintbrush, which comes with a reservoir of ink, onto my router mount and tried running the CamBam-generated g-code for the calligraphy of my name.  I set the 'cutter' angle to 35 degrees, to give a line width of about 5mm at full depth of, er, cut.

Seeing a paintbrush plunged to full depth in one go is excruciating to watch, and the end result was, to be generous, dreadful.  But strangely beautiful.  I love it!

Sorry, it will not happen again...

... unless someone comes up with a plug-in optimised for paintbrushes!  Hm!


Bob


Title: Re: V-Engrave Plugin
Post by: BR52 on February 04, 2014, 11:26:50 am
Hello Bob

What is important to also the diameter of the cutting tool V.
See here:
http://www.cambam.co.uk/forum/index.php?topic=3513.msg23559#msg23559

I have a theory, in place of the cutting tool you want to wear a paintbrush?
Please, you can put your DXF file here?

     Armando


Title: Re: V-Engrave Plugin
Post by: Garyhlucas on February 04, 2014, 15:31:33 pm
Er, OK, from the department of things that should never be repeated, I bring you - V-engrave with a paintbrush!

I rubberbanded a Pentel paintbrush, which comes with a reservoir of ink, onto my router mount and tried running the CamBam-generated g-code for the calligraphy of my name.  I set the 'cutter' angle to 35 degrees, to give a line width of about 5mm at full depth of, er, cut.

Seeing a paintbrush plunged to full depth in one go is excruciating to watch, and the end result was, to be generous, dreadful.  But strangely beautiful.  I love it!

Sorry, it will not happen again...

... unless someone comes up with a plug-in optimised for paintbrushes!  Hm!


Bob


Would that make it art?  We could make a fortune!


Title: Re: V-Engrave Plugin
Post by: macbob on February 04, 2014, 16:28:14 pm
Hi Armando,

I'm afraid I have not yet really got my mind round what 'diameter' means in the context of the V-Engrave mop.  I see the diagram in your thread, which implies that the diameter is measured at the point corresponding to the greatest depth to which you wish to cut.  However, I have got into trouble in the past with specifying a diameter and then finding that my value for Max Crossover Distance (0.7) caused the cutter to be transitioned from one zone to another below the surface depth.  Not good!  So recently I have been leaving the diameter as 0.

What is the benefit of specifying a diameter?

My paintbrush comes to a pretty good point and is basically a cone.  It can be 'plunged' by 8mm, at which time it is painting a mark 5mm wide.  Should I specify 5mm as the diameter?

My calculation of the angle 35 degrees came from 2 * arctan (2.5/8).

I would like to understand this, since I find the V-Engrave very useful, but I doubt I will be using a paintbrush again!

Bob


Title: Re: V-Engrave Plugin
Post by: BR52 on February 05, 2014, 20:25:14 pm
Hi Bob,

Only I will not put my plugin V_Corta in English is V_Cut

In reference to the diameter of the tool, I prove that this parameter is essential.
Install the "F-Engrave" and make several tests with different diameters.
Use the image below in .bmp for testing.

http://www.scorchworks.com/Fengrave/fengrave.html

       Armando


Title: Re: V-Engrave Plugin
Post by: BR52 on February 05, 2014, 20:56:52 pm
NOTE: Sorry did not yield to upload image of the "bmp" only ZIP file.

         Armando


Title: Re: V-Engrave Plugin
Post by: macbob on February 06, 2014, 02:58:52 am
H Armando,

I think I may be talking at cross purposes here; I used PSteMari's V-Engrave plugin, not your F-Engrave.

As far as I can see, the diameter of the cutter should make no difference, and this is also implied by his comment from the post following yours:

Quote
At any rate, none of that has any impact on the MOP or the toolpath.

I can see that the diameter of the cutter influences how wide a region may be cut without running the cutter so deep that it no longer reaches the boundary, but I believe that the V-engrave MOP does not take this into account.  I suppose it could fail if the boundaries were further apart than the diameter of the cutter, but I have not heard of it doing so.

My problem was that if you also specify the Max Crossover Distance, then the cutter diameter DOES come into play in determining whether the cutter should retreat to the clearance plane when transitioning from one region to another.  If it does not do so, the transition is not shown in red and is done below the level of the material surface. This happens even if two regions are not touching, but are closer together than 0.7 times the cutter diameter.  Setting either the cutter diameter or the Max Crossover Distance to zero stops this.

I regard this as a bug, but since the workaround is trivial, it is no big deal!  I find the V-engrave plugin a great addition to CamBam and have been using it quite frequently.

My post about the brush was basically just a joke - I was just trying it for fun to see what would happen!


Bob



Title: Re: V-Engrave Plugin
Post by: lloydsp on February 27, 2014, 01:04:11 am
Update on VEngrave.

Version b0006 with the MOp icon problem solved is here:
http://www.cambam.co.uk/forum/index.php?topic=4031.0

Lloyd


Title: Re: V-Engrave Plugin
Post by: BR52 on February 27, 2014, 14:47:49 pm
Hi Lloyd

Congratulations! you managed to solve the problem of Icons.
If I were you, I dismember the "Plugin.cs" file.
The "Plugin.cs" has many class into one file!

You mentioned:
// *****************************
// With apologies (because I couldn't get his permission to change this) and thanks to Paul,
// I've fixed the b0005 version for the MOp icon, and also fixed up the About text so that it's now version b0006.
// ******************************

In the source code you must comment on the author's name and your name as the modifier.
Cite the changes you did​​.

I would like to see the source code?

   Armando


Title: Re: V-Engrave Plugin
Post by: lloydsp on February 27, 2014, 15:05:29 pm
I did cite... in fact, I did not remove any of his citations, only adding mine as "modified on".

As soon as I have the chance to check the code for cleanliness (I add a lot of useless commentary during debugging), I'll re-post the source.  It's his, after all, and he deserves to see what fixed that problem.  Probably this evening, time permitting...

I would appreciate that you test to make sure I didn't damage some other part of his code.  I'm pretty careful about not changing anything but my targets, but you never know. <G>  There may be inherent bugs, but I don't want to have created any new ones.  Having both versions b0005 and b0006 would allow one to confirm or deny any new problems.

Lloyd


Title: Re: V-Engrave Plugin
Post by: lloydsp on February 27, 2014, 18:49:21 pm
Armando,
As a side note -- I am very dumb with C#... I still have no idea what many compiler directives do, and those confuse me greatly.  Additionally, CamBam.exe has many protected elements which cannot be explored with Reflector, and thus, I am at a disadvantage even to learn how it works.

That said, I know what you mean about having many classes in one source file, and I think I can 'cure' it in future.  Right now, though, I think any changes I make to Paul's code might break it.  The "changes" I made were simply to re-name some properties and generate a new gray-scale icon image.

What took the time was to understand how Andy had implemented the icons.  I gleaned that from the Threading MOp plugin, which is not so protected as to avoid exploring under Reflector.

Andy (as would any good 'binary' thinker) apparently thought of a "1" as "on", and a zero as "off".  Further, "enabled" is "on" and "disabled" is "off".

Extending that... his naming conventions for the icons make perfect sense -- the "1" suffix filename is the "on" image, and the "0" suffix the "off" image.   I _think_ I disagree with his doing it at all (I'm sure he had good reasons, though), because it would have been much more flexible to simply allow _any_ name for each image.

I will post the code.  However, knowing what I just told you, I'll bet you could fix up Paul's code as easily (ultimately) as I did.  The hard part was in the finding out how, not the fixing.

Lloyd


Title: Re: V-Engrave Plugin
Post by: lloydsp on February 28, 2014, 00:10:34 am
Here it is:

VEngrave plugin b0006 source.


Title: Re: V-Engrave Plugin
Post by: BR52 on February 28, 2014, 00:50:13 am
Lloyd you are an intelligent person.
 
Each compiler has algorithm of assembly and disassembly.
The ".NET Reflector" is an excellent decompiler.
Andy has every right to protect the source code mainly "CamBam.exe"

I suggest to Andy:
Create a few pages on the site of Cambam with secret password.
Transfer the purchase record for "CamBam.exe" file.
Unlock the "CamBam.CAD.dll" and "CamBam.Geom.dll" files.
The person who has unlocked these files are responsible.
Disclosure of those mentioned file is expressly forbidden.
The source code of the plugins will be put on the secret page.
One can not put on another site the source code.
Andy will have full control.

Written in Portuguese from Brazil.

Lloyd você é uma pessoa inteligente.

Cada compilador tem algoritmo de montagem e desmontagem.
O ".NET Reflector" é um excelente decompilador.
O Andy tem todo direito de preservar o código fonte principalmente do "CamBam.exe"

Eu sugiro ao Andy:
Criar algumas paginas no site do Cambam secreta com senha de acesso.
Transferir o registro de compra para o arquivo CamBamexe.
Desbloquear os arquivos "CamBam.CAD.dll" e o "CamBam.Geom.dll"
A pessoa que tiver estes arquivos desbloqueado são responsável.
É expressamente proibido a divulgação destes arquivo citados.
O código fonte dos plugins criados estarão na pagina secreta.
A pessoa não pode colocar em outro site o código fonte.
O Andy terá total controle.

   Armando


Title: Re: V-Engrave Plugin
Post by: lloydsp on February 28, 2014, 01:08:30 am
I'd love to see that, Armando, but it requires that Andy rely upon the honor of the person.  Unfortunately, he cannot discern that simply because someone purchases a license.  In fact, a person might do so simply to gain access to the source, and that would be to Andy's great detriment.  A 'contract' with the user is no guarantee, most especially because CamBam is sold across borders, and copyright laws vary from country to country -- especially having no value whatsoever in China.

Unless Andy publishes a compendium of methods and structures for the plugin programmer, I'm afraid we're limited to just poking around with test code and Reflector.

LLoyd


Title: Re: V-Engrave Plugin
Post by: lloydsp on March 03, 2014, 02:14:42 am
Arcs and circles (presumably) fixed.  Work it out hard, with innies, outies, circles, regions, polylines, segments, etc.

I've tested a few things which failed before, and they work now.

LLoyd
(attached below vb0007)


Title: Re: V-Engrave Plugin
Post by: BR52 on March 03, 2014, 19:31:18 pm
Lloyd

I did several test came back ok, you was very quick in the solution.
In MaxDepth properties I put in Auto frees the adjustment of tool diameter.
See the code in ComputeAutoMaxDepth() <---

As whistle I like see changes that you did​​.

   Armando


Title: Re: V-Engrave Plugin
Post by: lloydsp on March 03, 2014, 20:02:20 pm
Armando,
There were many changes I should have made to Math calls which used expressions for arguments, but I left them alone as "don't fix what isn't broken".

Instead, except for documenting by comments, I made only ONE tiny change to geometry.cs, in the RadiustoArc subroutine, vis (look for AHAH!):

    public static double RadiusToArc(Point2F position, Vector2F normal,
                                     Point2F start, Point2F end,
                                     double bulge) {
      // Figure out which side of the (start,end) vector we're on from
      // the cross product of (start->current)x(start->end).
      // + is on the right.
      var darc = new Vector2F(start, end);
      var dsp = new Vector2F(start, position);
      // Precondition: Math.Abs(bulge) >= DBL_EPSILON
      // Compute arc center and radius
      Point2F arcCenter;
      double arcRadius = ConvertBulgeToArc(start, end, bulge, out arcCenter);
      // and from that the cross products of the vectors from the center
      // to start and position, and to the position and end
      Vector2F dpc = new Vector2F(position, arcCenter);
      // Compute tangent circle
      double radius;

      // Common values
      double normalDotCenterMinusPos = Vector2F.DotProduct(normal, dpc);
      double distanceToCenter = dpc.Length;

      int directionToContactPoint;    // +1 to towards arcCenter, -1 if away
      Point2F contactPoint;
      if (Math.Abs(distanceToCenter - arcRadius) < DBL_EPSILON) {
        // then the point is on the circle defined by the arc.
        directionToContactPoint = 0;
        radius = 0.0; // Unconstrained if normal is perpendular to arc
        contactPoint = position;
      } else {
        double distanceToCenter2 = distanceToCenter*distanceToCenter;
        if (distanceToCenter2 < arcRadius*arcRadius) {
          // then we're inside the circle and have the concave case
          double denom = 2*(arcRadius - normalDotCenterMinusPos);

/*AHAH!!!! this 'ergo' by Paul, below, does not hold true!  denom CAN be zero, and that causes a divide-by-zero failure
   with circles and some arcs.
*/
// per Paul...
          // normal . (C-P) < |C-P| < Ra, ergo denom != 0

/*  SO... this fix... which has to be tested with 'funny' arcs, not just circles  03/02/2014 by L.E.S.
       It is always postive because radius is always an absolute value, and is computed below from two squares,
       which by definition are always positive.  I could have just added DBL_EPSILON to the denom calculation
       above, but that would slightly change EVERY calculation, not merely when denom=0... just bad practice.
*/
          if (denom==0) {
           denom=DBL_EPSILON;  // smallest value a double can be
         }
//  End of AHAH!


          radius = (arcRadius*arcRadius - distanceToCenter2)/denom;
          directionToContactPoint = -1;
        } else {
------------------------------------------

Lloyd


Title: Re: V-Engrave Plugin
Post by: Bubba on March 04, 2014, 00:47:48 am
Work it out hard, with innies, outies, circles, regions, polylines, segments, etc.
+++++++++++++
You asked, I did..


Title: Re: V-Engrave Plugin
Post by: lloydsp on March 04, 2014, 01:32:11 am
Well, that doesn't look very good, Bubba, but I think you forgot something.

Those 'double' circle/oval shapes must be converted to regions to work with VEngrave.  Always did.  Otherwise, you just diddle out the whole circle, instead of the gap between the two.

This is what it's supposed to look like... <G>


Lloyd


Title: Re: V-Engrave Plugin
Post by: Bubba on March 04, 2014, 13:22:49 pm
Those 'double' circle/oval shapes must be converted to regions to work with VEngrave.
+++++++++++++

Thanks for point it that out Lloyd. I wasn't aware of it.

It does look good. Thanks.


Title: Re: V-Engrave Plugin
Post by: macbob on March 04, 2014, 15:10:56 pm
Hi Lloyd,

I believe that this is all working perfectly now!

I attach the first case where I encountered this problem.  It used to run for 30 minutes and then stop with the floating point problem.  It now finishes perfectly in about an hour and a half!  This might be a good test case, although only as a last resort!  The Inlay>>V-Engrave MOP is the larger one.

[This project was a work in progress that I was just playing with during experiments with inlays - it is not suitable for actually carving, and may never be, because I no longer like the pattern!  Too cutesey!]

Many thanks for picking up this ball and running with it!

Bob


Title: Re: V-Engrave Plugin
Post by: lloydsp on March 04, 2014, 15:27:36 pm
Heh!  Yeah on the "cutesie", and yeah on how long it must take to run!  Dang!  That's a lot of detail for VEngrave to pick through one 'resolution width' at a time!

That would probably take quite a while to do even with simple pockets.

You're quite welcome; but understand, I did it mostly out of a personal musterbation to learn C# and the VS tools.  That it's of general benefit just makes it all the more fun<G>.

LLoyd


Title: Re: V-Engrave Plugin
Post by: macbob on March 10, 2014, 02:51:55 am
Hi Lloyd,

I'm sorry, but even with your new plugin version, the attached file's first MOP gives me the dreaded "Not-a-number" alert when I generate toolpaths.

I tried your trick of resizing trivially in one axis or the other, to no avail.  Sigh!  This is again a rather convoluted shape - perhaps I need to stick to simpler outlines!

Bob


Title: Re: V-Engrave Plugin
Post by: pixelmaker on March 10, 2014, 10:30:50 am
hello
I get the message

Processing segment[18], starting point: 179.914, 223.291, 0 B 0
Primitive 0[18] is too short


ralf


Title: Re: V-Engrave Plugin
Post by: lloydsp on March 10, 2014, 11:38:09 am
Both... I will look at the code and see if I can identify where that's coming from.  There are a LOT of calls to the Math library in there that presume all the parameters will be correct, without testing them first.  That's an invitation to future discoveries of bugs.

I eschewed changing them in favor of fixing the only _known_ bug  -- at the time.  I guess it's time now to fix all of those calls to prevent this sort of thing from cropping up in future.

LLoyd


Title: Re: V-Engrave Plugin
Post by: lloydsp on March 10, 2014, 14:13:42 pm
Ok... I've found the offending segments in the Floral Swirls pattern, and my opinion is that there's nothing wrong with them.  So, again, this is a math precision thing, with the likelihood of yet another divide-by-zero encounter.

I'll find it.  Probably this evening.  Maybe I'll just wash the whole body of code for that sort of dirt.

LLoyd


Title: Re: V-Engrave Plugin
Post by: lloydsp on March 10, 2014, 19:54:45 pm
OK, here it is MacBob.

I didn't fix everything, because that's going to take a LONG while to discern what needs fixing, but I did find your issue.

Paul was testing to see if a segment was too short to process within the precision of the math he was using.  If so, he issued a warning about it, then continued doing the math that HAD TO FAIL due to a division by zero.

So, actually, this was not a divide-by-zero issue, but a failure to exempt the segment in question from being drawn.  Hey... if it's too small to compute, it's too small to MILL.  So I added a 'skip' feature for those.

It will still report the warning at the right messages level, but will say it's skipping it, instead of just telling you it's too short to process.

V b00008. 

I ran both your substrate and inlay patterns all the way to g-code.  The substrate took about 00:01:37 to run, and the inlay about 00:02:15... and that was on my piggy laptop in the shop, so it should run quickly on any modern PC.

Attached.

LLoyd


Title: Re: V-Engrave Plugin
Post by: macbob on March 10, 2014, 20:34:29 pm
Wow!  Thanks for the instantaneous response!

I will download that when I get home from work and see how it goes, although I'm sure that if it works for you it will work for me.

I had used 'Clean' and 'Remove Overlaps' on my path - perhaps one of these should automatically remove line segments that are too small to be useful?

Many thanks,

Bob


Title: Re: V-Engrave Plugin
Post by: lloydsp on March 10, 2014, 20:45:33 pm
Heh!  I guess that might work, but now that the software accommodates it... why bother?

Besides, in this case, it was not one of YOUR line segments, but rather, the 'internal' primitives of the toolpath that Paul develops in the code.  So there's not much you could have done about it, nor Andy.  The only way to solve it is to detect it and skip the segment.

I might add this:  It's a LOT easier to find a known bug than to find ones you don't know about, so your testing is very valuable.  

I don't intend to sound condemning or mean-spirited about Paul's work -- it was AMAZING!  Bugs can't always be anticipated.  THIS one could have been, though, because he'd already tested for it. <G>

Lloyd


Title: Re: V-Engrave Plugin
Post by: macbob on March 11, 2014, 00:36:27 am
Excellent - Works perfectly for me too.

I see your 'skip' message.  Interestingly, only once.  I must have been unlucky, or lucky, depending on your point of view.

I think that if the segment referred to is not mine, then the message conveys no information to an end user.  In the long term, once you have things stable, it should probably just be suppressed.

I am starting to get confident with inlays - now I gotta stop downloading dubious internet clip-art and start designing something I actually like  ;D. 

Thanks again,

Bob




Title: Re: V-Engrave Plugin
Post by: lloydsp on March 11, 2014, 01:09:47 am
Bob,
I agree.  Your two inside-profile segments (good ones) landed at such an angle and distance relative to the outer profile of that region so that the 'turn' about the sharp corner had one zero-length arc in it.  Right now, I just want to see how often it occurs.  Something might be done to lower the precision of the math to something more resembling the real-life movements of a mill, and I think it would save processing time, too.

I have one question.  I don't quite understand the relationship of the engraving on both the substrate and inlay.

Do you have a photo or concept drawing of how that FloralSwirl thing is supposed to work and look? Or was that just a 'test case'?

Thanks,

LLoyd


Title: Re: V-Engrave Plugin
Post by: macbob on March 12, 2014, 17:19:20 pm
I'm afraid that what I sent you was just a work in progress, and probably not one going anywhere much either.
The inlay cut needs to be mirror-imaged and it is completely missing the roughing part that cuts out the bits in the middle of both substrate and inlay.

I have been playing around with inlays to try to get my mind round it.  The simple cases are easy and the cases where the pattern has complex regions are more tricky.  I have some notes for myself - I will try to pull them together and put them out on the forum.

Bob


Title: Re: V-Engrave Plugin
Post by: atwooddon on March 12, 2014, 18:01:55 pm
There are several applications for this 'double bevel' for inlays.  Here is a YouTube video describing one way of doing the double bevel inlay to allow the very fine end points for a shape.  There several other ways of doing this, only listing this one as it the first I have been able to find easily.

https://www.youtube.com/watch?v=d4992bEoNYI

I saw an article a couple years ago about using a cnc machine doing similar work, but with much thinner pieces of contrasting woods to create the inlay and then the thin inlay veneer was glued to a substrate.  Haven't been able to find the article right now.

Don


Title: Re: V-Engrave Plugin
Post by: lloydsp on March 12, 2014, 19:18:08 pm
Don, to my knowledge, all "fine" woodworking inlays were done with a bevel in the classic furniture era.  When I was pursuing that art, we cut them with a very slightly-tapered cutter -- only a degree of cant.

It has the advantage of jamming tightly into the socket, and compressing the edges to the point of making the seam vanish.

LLoyd


Title: Re: V-Engrave Plugin
Post by: BR52 on March 13, 2014, 01:19:09 am
Lloyd
Please, you can put the source code for version B0008.

   Armando


Title: Re: V-Engrave Plugin
Post by: lloydsp on March 13, 2014, 10:42:54 am
Armando,
Again in the interest of not posting a bunch of files for a one-line change... here is the information.

There is only ONE tiny code change: the addition of a "continue" to a test Paul had already made. Then the message has been changed from Warning level to Debug level to prevent it's issuance normally, and of course, comments were entered in the head of the file.

All this is in "plugin.cs", and is detailed below:

In the running commentary at the head of the file, this is added:

" On 3/10/14, MacBob found another one.  When Paul processed a segment too short to do any math
 upon, he issued a warning message, but didn't skip that segment.  As a result, he ended up
 with an N/A value in the structure "dse" down in the FollowOutline routine.  Look for the "OOPs!" in
 FollowOutline in Plugin.cs (this file).
 */

And this in the "FollowOutline" procedure:  just search for the "If (len < DBL_EPSILON)", which is unique in this file.

      if (len < DBL_EPSILON) {         
           // the Warning message changed 3/10/14 to something meaningful.  LES
           //_log.Log(WARNING, "Primitive {0}[{1}] is too short.", outline.ID, i);
           // message level is changed so the user doesn't usually see it, since it refers to internal operations
           
          _log.Log(DEBUG, "Primitive {0}[{1}] is too short to cut, so it is being skipped.", outline.ID, i);

          //  OOPs! Paul didn't skip it!!... if it's zero length or too short to process,
          // then it's ALSO too short to mill... SKIP the segment instead of just issuing warnings!
          // Failure to skip the segment almost guarantees a math error or undefined result.  LES 03/10/14
 
//  Add this code change to skip the segment ---
           continue;   // don't abandon the whole outline, just this one segment -- added 3/10/14 LES
 //  End modification 3/10/14

         }
         

LLoyd


Title: Re: V-Engrave Plugin
Post by: BR52 on March 17, 2014, 15:31:39 pm
Hi Lloyd

Please, see attached file for analysis.
And see code snippet, has no function?

Code:
internal void ComputeCutEndcap(
      Point3F endpoint, Vector2F openDirection, SurfaceBuilder bob) {
      //double bottomRadius = ToolTipDiameter.Cached/2;
      //double topRadius = bottomRadius + (StockSurface.Cached - endpoint.Z)*Math.Tan(0.5*ToolVAngle.Cached*DEGREES); // <---
      //double endAngle = openDirection.Normal().Angle;
      //double startAngle = endAngle - Math.PI;
      //int nPoints = Math.Max(8, (int) (Math.PI*topRadius/PathIncrement.Cached));    // <---
      //
      //Point3F prevTop = new Point3F(
      //  endpoint.X + topRadius*Math.Cos(startAngle),
      //  endpoint.Y + topRadius * Math.Sin(startAngle),
      //  StockSurface.Cached);
      //Point3F prevBottom = new Point3F(
      //  endpoint.X + bottomRadius*Math.Cos(startAngle),
      //  endpoint.Y + bottomRadius*Math.Sin(startAngle),
      //  endpoint.Z);
      //for (int i = 1; i <= nPoints; ++i)
      //{
      //    double angle = startAngle + i * (endAngle - startAngle) / nPoints;
      //    Point3F currTop = new Point3F(
      //      endpoint.X + topRadius * Math.Cos(angle),
      //      endpoint.Y + topRadius * Math.Sin(angle),
      //      StockSurface.Cached);
      //    Point3F currBottom = new Point3F(
      //      endpoint.X + bottomRadius * Math.Cos(angle),
      //      endpoint.Y + bottomRadius * Math.Sin(angle),
      //      endpoint.Z);
      //    bob.AddFacets(prevTop, prevBottom, currBottom, currTop);
      //    prevTop = currTop;
      //    prevBottom = currBottom;
      //}
    }
     
   Armando



Title: Re: V-Engrave Plugin
Post by: lloydsp on March 17, 2014, 15:40:36 pm
Armando,

I'm not clear what you're saying.  ComputeCutEndCap() is not commented out like that in the versions I have.

Did you nullify it, or does your code have it that way already?

It does, indeed do _something_, since it alters certain globals during its execution.  I have not studied it to see what effect it has, but I never modified it.

Lloyd


Title: Re: V-Engrave Plugin
Post by: BR52 on March 17, 2014, 17:37:14 pm
One of the ways to see some of the functions is make comment to nullify its effect!
Inside of a function procedure, if have to a call function, careful to make comment to this function call.

What is important you look at the file that I put.

   Armando


Title: Re: V-Engrave Plugin
Post by: lloydsp on March 17, 2014, 17:44:54 pm
Ok, I don't have time to modify and re-compile my own copy right now.

Obviously, you've shown another bug.  If you remove the "end cap" function, does the errant toolpath go away?

Also, how can you be certain the function has no purpose or effect?  Might it not be important in some other shapes?  (Since I have not evaluated what it does, I only know from looking that it does modify some terms, so it does NOT have "no purpose", even if that purpose is buggy.)

I'm still confused as to the point of your comment.  Explaining in more detail would help me understand.

LLoyd


Title: Re: V-Engrave Plugin
Post by: BR52 on March 18, 2014, 01:34:20 am
Lloyd,

The "Analise2.cb" file has a bug, he has nothing to do with ComputeCutEndcap.
I called your attention to:
ComputeCutEndcap(Point3F endpoint, Vector2F openDirection, SurfaceBuilder bob)

It is also considered as:
      "A method that does not return a value cannot be verified."

   Armando


Title: Re: V-Engrave Plugin
Post by: lloydsp on March 18, 2014, 10:17:36 am
Ok... I guess language is getting in the way, or else I'm not astute enough to understand.

ComputeCutEndCap does not return "a value", it creates facets.  It does something very tangible, just not in terms of passing back something to the caller.  That may be 'bad practice', but it's commonly done.

I do not understand your purpose in commenting-out certain sections of it.  Surely that changes what it does, but to what end?  Do you know when the method is being called?  Have you added log outputs to it to see when and what effects your changes have?

I'm struggling to understand your purpose; maybe if I had time to evaluate it myself, I could.

LLoyd


Title: Re: V-Engrave Plugin
Post by: dsnellen on April 28, 2014, 14:13:17 pm
The plug-in works great. Is there a way to implement the Depth Increment option in the cutting MOP? I use a 30 degree engraving tool and having it cut at a depths greater than 0.25" is a bit much. Thanks.

Dave


Title: Re: V-Engrave Plugin
Post by: atwooddon on April 28, 2014, 15:48:27 pm
As a work around, you can make 2 mops, the first with a flatter cutter angle (ie 60 degrees) which will prevent the 30 degree bit from going as deep then make a second mop using the 30 degree setting.  Try it in CamBam, look at a side view of the cuts and you will see it cuts shallower with the 60 degree setting than with the 30 degree setting.

Don


Title: Re: V-Engrave Plugin
Post by: lloydsp on April 28, 2014, 16:52:08 pm
In any case, remember that because of the way the V-engrave plugin works, you'll RE-engrave ALL of the lines, if you use a 'depth increment', whether added as a feature, or using that (smart) idea of changing the cutter angle.

The way it's written now, it cannot simply go back over the deeper parts.  It will cut 'air' in all the shallow areas on the second pass, if only a simple depth increment is implemented in the code.   At least with the 'trick' Don suggested, it will cut on both passes, satisfying your emotional need to see metal moved on every pass <G>.

I think there could be some (difficult) code written to find the deeper areas, and engrave only those, but it would be a large task.

LLoyd


Title: Re: V-Engrave Plugin
Post by: atwooddon on April 28, 2014, 16:59:11 pm
Agree with Lloyd's comments.  I have tried playing with the depth increment by actually starting with the bit above the material so only the deeper parts of the engraving are cut but it just turned out to be easier to cut in multiple passes by 'fudging' the bit angle.  Simple trick but it does double the carving time when you use it.

Don


Title: Re: V-Engrave Plugin
Post by: dsnellen on April 28, 2014, 17:28:14 pm
Thanks for the suggestion. I used the dual MOP idea. Cutting now.
Dave


Title: Re: V-Engrave Plugin
Post by: billt on April 29, 2014, 01:33:27 am
A minor issue maybe you guys would be willing to investigate?
The start/end points do not connect when they are located on a straight section or "smooth" corner.
This effect is apparent when the step size is large (see attached screenshot).
As a fix, step size can be decreased (increasing processing time), or the start point moved to a sharp corner, but neither of these are ideal.

The issue is logged as issue #17 in pstemari's google code site for V-engrave.
https://code.google.com/p/v-engrave-plugin/issues/detail?id=17
He suggests on Post#11 that the pruning of the start/end points occurs at line 1205 (rev 0005)

Thanks!  BillT


Title: Re: V-Engrave Plugin
Post by: dsnellen on April 29, 2014, 02:02:52 am
The 2 MOP idea works really well but does double the cutting time. Learning the cutter angle controls the depth of cut, I also tried a 45 degree. It worked really well with the 30 degree cutter. The depth was around 0.20 which which is acceptable. The letters are slightly narrower, but still crisp and sharp. This is a great little plug-in.

David


Title: Re: V-Engrave Plugin
Post by: mikek on April 29, 2014, 19:44:11 pm
Hi All,  How do I get tool params set properly for CutViewer?

I've created a V-Cutter in my Tool Library->Default-in library. But I see wrong/incomplete parameters being used
in my .nc file's TOOL/MILL line. Here's an example:

In my Tool Library's Tool Geometry I have(in inches):
Diameter: 0.5
Flute Length: 0.5
Flutes: 2
Helix Angle: 0
Length: 1.5
Shank Diameter: 0.25
Tool Profile: V-Cutter
Vee Angle: 80

What I see in the .nc line is this:
(  TOOL/MILL,0.5,0.0,1.5,0  )

So CamBam (or V-Engrave Plugin?) are placing the Overall Length parameter in place of
Flute Length even though the tool def has Flute Length called out. And, the Taper Angle is just set to
zero even though there's all the info needed to calculate it (Vee Angle/2) and provide it.

I've tried two versions of V-Engrave Plugin b0004 and b0007.  They both do the same thing.
Is this a Cambam issue, a V-Engrave issue, or a Mike issue? :)

Another item. In my first runs I had forgotten to set the Post-Processor to Mach3-CutViewer and so got
no tool setup lines.  No problem I wasn't using CutViewer at first. Then, when I discovered the lack of
tool and stock in CutViewer I made that change to the Post Processor entry and tried re-generating toolpaths
and re-creating nc, but I found that the tool/stock info was still missing from the nc code and I had to
save the design and rerun toolpaths and nc to get the change noticed. I don't recall having to save before
creating nc, although is IS recommended in the manual. The manual does not say it's required.

Mike


Title: Re: V-Engrave Plugin
Post by: mikek on April 29, 2014, 19:52:37 pm
Relying to my own post,

I see that according to CutViewer manual the TOOL line in the nc should likely be a
TOOL/CHAMFER rather than TOOL/MILL. But the issue is still the same. I'm see incorrect
TOOL statements in the nc.

Mike


Title: Re: V-Engrave Plugin
Post by: mikek on May 09, 2014, 06:12:32 am
While waiting for our power users and Andy to enhance Cambam to correctly generate CutViewer
TOOL statements for Engrave MOPs I have found a temporary fix.
Only tested when using the Mach3-CutViewer Post Processor.

Select the Engrave/VEngrave MOP.
Add the following five lines (at least the last line) to the "Custom MOP Header" parameter under G-Code Options.

{$comment} CUTVIEWER addon by Mike Kirkpatrick for Engrave MOPs {$endcomment}
{$comment} This addtion sets the tool correctly for CutViewer for V-Cutters. {$endcomment}
{$comment} Add these lines to "Custom MOP Header" parameter in the G-Code Options section." {$endcomment}
{$comment} Add these lines to the Engrave/VEngrave MOPs only. {$endcomment}
{$comment} TOOL/CHAMFER,{$tool.diameter},{$tool.veeangle},{$tool.length} {$endcomment}

I just keep these lines in a file and copy/paste into the edit field when needed. Kinda clunky but does the job.

Mike


Title: Re: V-Engrave Plugin
Post by: pixelmaker on May 09, 2014, 10:14:13 am
Mike

in your used postprocessor in the line "Tool Change" put a {$tool.comment}, like :
{$clearance}{$tool.comment}
{$comment} T{$tool.index} : {$tool.diameter} {$endcomment}
T{$tool.index} M6


In your tool library you use now the line "Comment" for the {$tool.comment}. For a endmill or ballnose cutter you use the pattern:
{$comment} TOOL/MILL,{$tool.diameter},{$tool.radius},{$tool.length},0 {$endcomment}
{$comment} COLOR,150,255,0 {$endcomment


for a V-cutter you use the pattern:
{$comment} TOOL/Chamfer,{$tool.diameter},90,{$tool.length},0 {$endcomment}
{$comment} COLOR,80,220,0 {$endcomment}


If you write this comments in to your tool library you not need to copy something in to your mop.
The variable {$tool.comment} writes the values from your tool library into the g-code

ralf


Title: Re: V-Engrave Plugin
Post by: mikek on May 09, 2014, 17:48:37 pm
Hi Ralf,

I was hoping someone would come back with a more elegant solution. I appreciate your help.

The Mach3-CutViewer post processor already has all but the {$tool.comment} in the
<ToolChange> section. In particular it already has an entry that produces TOOL/MILL lines
used for end mills and ball mills WITHOUT having to add comments to any of those tools in the tool libraries.
I like to keep changes to the minimum.
So I just added the new {$tool.comment} in the post processor just below the existing TOOL/MILL line
and then any special tools that have comments defined in the tool libraries will win out in CutViewer.

One point of correction though...

The CutViewer manual gives the following two options for CHAMFER tools.
   TOOL/CHAMFER, Diameter, Point Angle, Height
   TOOL/CHAMFER, Diameter, Point Angle, Height, Chamfer Length

I use the first one for V-Cutter tools. I discovered by guessing that the "Point Angle" can be supplied
a value via the variable {$tool.veeangle}. This works to provide the Vee Angle as defined in the tool library.

Mike


Title: Re: V-Engrave Plugin
Post by: pixelmaker on May 09, 2014, 18:31:17 pm
Quote
So I just added the new {$tool.comment} in the post processor just below the existing TOOL/MILL line

If your pp has  already  the {$tool.comment} in the  <ToolChange> section you must not insert a second one.
The {$tool.comment} prints the comment line of the tools in the library in the code no matter what is entered there.
For a V-cutter you can use a line
{$comment} TOOL/Chamfer,{$tool.diameter},{$tool.veeangle},{$tool.length},0 {$endcomment}
{$comment} COLOR,80,220,0 {$endcomment}

I know no variable for the chamfer lenght in Cambam. Instead of the 0 this value must write in the tool library comment line by hand.

ralf


Title: Re: V-Engrave Plugin
Post by: lloydsp on May 09, 2014, 19:33:34 pm
I have to add this thought:  That seems to me to be a VERY elegant solution.

It uses the 'fixed' properties of the tool libraries and post processor.  It follows the TOOL and not the MOp.

It does not require that you muck up your individual MOps with excess, custom stuff that would be difficult to properly document and duplicate.

I have to give "hats off" to Ralf for coming up with that solution.

I didn't ever see it as possible, and I will implement it as soon as time permits.

Lloyd


Title: Re: V-Engrave Plugin
Post by: jerrywi on May 25, 2014, 13:25:39 pm
Down loaded plugin yesterday, FANTASTIC. Thank you so much.
Jerry


Title: Re: V-Engrave Plugin
Post by: dh42 on July 08, 2014, 16:07:05 pm
Hello,
A friend has a problem to install the Vengrave plugin.

An idea of what is going wrong ?

(http://i39.servimg.com/u/f39/16/50/61/19/08_jui16.jpg)

++
David


Title: Re: V-Engrave Plugin
Post by: lloydsp on July 08, 2014, 16:22:18 pm
David,
It sort of smells like he needs to change his graphics mode in CB.

LLoyd


Title: Re: V-Engrave Plugin
Post by: dh42 on July 08, 2014, 17:16:36 pm
Hello,

Quote
It sort of smells like he needs to change his graphics mode in CB.

Yes, I told him to swith to OpenGL_legacy ... but I doubt that is what disturbs loading Vengrave ... wait and see ..

++
David


Title: Re: V-Engrave Plugin
Post by: dh42 on July 08, 2014, 17:43:41 pm
More infos after tests.

- system is Win XP
- Cambam version is 0.9.8 N
- The other plugins works
- same error with the plugin after changing the OpenGL_mode.

(http://i39.servimg.com/u/f39/16/50/61/19/sans_t19.jpg)

 ??? ???

++
David


Title: Re: V-Engrave Plugin
Post by: lloydsp on July 08, 2014, 18:07:01 pm
If he did not compile this himself, and is only attempting to run the V.0008 .dll, then there are some system .dlls that might need updating.

The list in the source is:
using System;
using System.Collections.Generic;
using System.ComponentModel;
using System.IO;
using System.Runtime.CompilerServices;
using System.Windows.Forms;
using System.Xml;
using System.Xml.Serialization;

I do not know, off hand, which system .dlls correspond to those functions, but if there's a version mismatch between what it was compiled under and what he's running, that would explain the exception being thrown.

LLoyd


Title: Re: V-Engrave Plugin
Post by: dh42 on July 08, 2014, 18:16:05 pm
Maybe problem found ; he don't have the net 3.5 ; only net 2.0 ...

I thought that cambam don't works at all if the net 3.5 are not here .. but it works ..

++
David


Title: Re: V-Engrave Plugin
Post by: lloydsp on July 08, 2014, 18:55:54 pm
I don't know.... some of my plugins are written specifically around .Net 3.5 calls.  I wouldn't trust them to work with prior versions.  I imagine it partly has to do with how many functions of CB he's tried so far.  Maybe it applies only to extensions and plugins. ???

LLoyd


Title: Re: V-Engrave Plugin
Post by: dh42 on July 08, 2014, 19:01:30 pm
Ok, answer tomorrow ... (4 hours to download .. net 3.5  ::))

++
David


Title: Re: V-Engrave Plugin
Post by: pixelmaker on July 08, 2014, 19:08:09 pm
hello David

this "erreur de verification du version" means only that cambam can´t connect the cambam.co.uk to detect if the installed version is the newest version. This is only a www connection problem and has nothing to do with the other errors. If the connection is ok you get a "you have the actuall cambam version installed". You can switch it off in the options. Perhaps the computer has no connection to www.
The other errors depends of the graphic board.
Your friend should reinstall the driver for the graphic board.
Try OPEN GL with the GLSL_110 shader in the options

ralf



Title: Re: V-Engrave Plugin
Post by: dh42 on July 08, 2014, 19:14:44 pm
Hello Ralf ;)

Yes I know, and this two errors are solved ... only the pb with the Vengrave plugin is still here ...

++
David


Title: Re: V-Engrave Plugin
Post by: dh42 on July 08, 2014, 21:28:48 pm
re

Problem solved ; it was the .net 3.5 ...

++
David


Title: Re: V-Engrave Plugin
Post by: EddyCurrent on August 16, 2014, 20:05:17 pm
I decided to get the CutViewer issue sorted.

This is the normal result

( Made using CamBam - http://www.cambam.co.uk )
( v9 8/16/2014 3:55:45 PM )
( T15 : 23.0 )
( CUTVIEWER )
( FROM/0,0,5 )
( Select dummy tool to avoid warnings )
( TOOL/MILL,1,0,20.0,0 )
( STOCK/BLOCK,,,,,, )
G21 G90 G91.1 G64 G40
G0 Z3.0
( T15 : 23.0 )
( Tool Taper coming soon )
( TOOL/MILL,23.0,0.0,20.0,0 )
T15 M6
( VEngrave1 )

and this is how I have it now

( Made using CamBam - http://www.cambam.co.uk )
( v9 8/16/2014 7:16:49 PM )
( T15 : 12.0 )
( CUTVIEWER )
( FROM/0,0,5 )
( Select dummy tool to avoid warnings )
( TOOL/MILL,1,0,20.0,0 )
( STOCK/BLOCK,,,,,, )
G21 G90 G91.1 G64 G40
G0 Z3.0
( T15 : 12.0 )
( Tool Taper coming soon )
( TOOL/CHAMFER,12.0,60.0,20.0,0.0 )
T15 M6
( VEngrave1 )

This is what I did.

1. Created a new tool in the Default-mm section.
2. Entered details for Flutes, Length, Tool Profile, Vee Angle
Length was set to 20.0 just because it's a reasonable value.
Vee Angle was set to 60.0 degrees but the idea is to create more tools with different angles so when setting up a new V-engrave MOP the correct tool can be selected.
3. Changed 'Tool Name Format' to {$diameter}mm {$flutes} flute {$profile} {$veeangle} deg
4. In the newly created tool 'Tool Change' field I entered this;

{$clearance}
{$comment} T{$tool.index} : {$tool.diameter} {$endcomment}
{$comment} Tool Taper coming soon {$endcomment}
{$comment} TOOL/CHAMFER,{$tool.diameter},{$tool.veeangle},{$tool.length},0.0 {$endcomment}
T{$tool.index} M6

These lines override the post processor tool change property.

Now when a new V-engrave MOP is set up the user has to enter the Tool data as normal but be sure to select a new tool that matches the vee angle entered, in this example Tool index 15

CutViewer now works correctly.

It's a pity the Tool Tip Diameter can't be passed to the TOOL/CHAMFER line, the assumption for CutViewer is that all tools come to a point i.e. Tool Tip Diameter = 0


I made a spreadsheet to calculate the dimension L (chamfer length) for this format;
TOOL/CHAMFER,Diameter,Point Angle,Height,Chamfer Length
By entering the tool diameter,vee angle,tool tip diameter the value for L is calculated and can be manually typed into the the Tool Change field text instead of 0.0 as shown above.


Title: Re: V-Engrave Plugin
Post by: GeoffreyGRoy on September 03, 2014, 10:54:03 am
I have noted some strange behaviour when viewing MOPs from the V-Engrave plugin.  The MOPs seems to be correct (i.e the geometry is correct), but when I rotate the view, the apparent Z-position of the cut paths seems to rapidly increase in the -Z direction - when the position of the original objects are placed below the stock surface.  As far as I can tell it is just a viewing issue, not an actual geometry issue.

In the attached images, image1 is a plan view of an MOP created from V-Engrave with the letter object at Z=-3.  If I rotate the image just a wisker I get image2 - the cut paths disappear rapidly to a large -ve Z while the geometry object rotates correctly.


Has anyone else noted this behaviour?

Geoff


Title: Re: V-Engrave Plugin
Post by: pixelmaker on September 03, 2014, 12:25:20 pm
Geoffrey,
as I remember the toolpath always starts at Z=0, , even if the original object has a different Z-height.
If you set a lower Stock Surface in the v-engrave mop the toolpath rapids down to the start of the cut, also if the start of cut is lower then Z=0.


ralf


Title: Re: V-Engrave Plugin
Post by: GeoffreyGRoy on September 04, 2014, 10:02:47 am
Dear Ralf

That is probably the case, but not the problem I have found - it is just a viewing problem - I think.

 I have used the plugin to create my MOP and actually cut it without problems.

Geoff


Title: Re: V-Engrave Plugin
Post by: pixelmaker on September 04, 2014, 11:38:53 am
Geoff
I can´t see any viewing problems. I looked for it but all is ok.
I use a orthographic view.

ralf


Title: Re: V-Engrave Plugin
Post by: sraney on September 04, 2014, 21:04:20 pm
Great Plugin. But I seem to have found an odd issue with memory while generating the toolpaths.  I've pulled the parts apart and reviewed them and can not see a problem with it.

VEngrave7 (Polyline182) is the first one I located. I have even pulled it into a new file and attempted to just generate tool paths for it.  VEngrave15 (Polyline186) also produces the same issue.

(http://i57.tinypic.com/zv3536.jpg)

 I've attached the CB file



Title: Re: V-Engrave Plugin
Post by: EddyCurrent on September 04, 2014, 21:59:19 pm
VEngrave15 works fine for me but 7 takes longer then I care to wait, in fact I did not see it complete.
Also there is no MOP for Polyline (182)
I cut the Polyline (186) into two pieces and each half completed no problem, can't see why it's no good as one line.


Title: Re: V-Engrave Plugin
Post by: pixelmaker on September 05, 2014, 00:47:37 am
hello
first use the -> edit -> polyline -> arc fit with value 0.01 to reduce the nodes.
Then I create a new active layer
Select Polyline 186 and use -> edit -> polyline -> remove overlaps with value 0.01
A new polyline (1) is created at the new layer
Use this polyline (1)  in VEngrave7 without problems.

If you work with dirty files you have to clean the polylines first.

ralf


Title: Re: V-Engrave Plugin
Post by: pstemari on September 06, 2014, 23:03:24 pm
Sorry I didn't see this earlier.  Been busy with other things and my engraving project was interrupted by a change of product logo at work.

Yes, the circle is an edge case and I haven't added any code to explicit support it.  There's some optimizations applied to the g-code that remove superfluous points from the toolpath, basically duplicates or points that lie within a tolerance of the line between adjacent points.  What that means for a circle is that all the points are duplicates and get optimized away (good), but that the one remaining point is tossed out (not good).

I'll take a look to see what's involved with a fix.  I don't know off-hand if the remaining point is getting thrown out by my code or CamBam's code.

As far as i18n goes, I don't have any code to explicitly support it.  If anything is happening at all, it's because of underlying support in CamBam. 



Title: Re: V-Engrave Plugin
Post by: pstemari on September 06, 2014, 23:35:30 pm
Circles: http://code.google.com/p/v-engrave-plugin/issues/detail?id=20
i18n: http://code.google.com/p/v-engrave-plugin/issues/detail?id=21

I'll also be moving the project over to GitHub sometime in the next few weeks; I will keep you all posted on that.

Tip diameter:  v-bits normally have a small flat on the end.  If you don't adjust for this all the engraving will be too wide by the diameter of the tip.  On a small engraving bit that becomes very important:  0.005" on a 0.010" wide line is pretty noticeable!  On routers making big signs in wood, just set it to zero and don't worry about it.

I like the angle adjustment for depth.  The issue I was struggling with for doing multiple passes was how to make a smooth final pass and avoid any steps.  The angle adjustment just applies a scale factor to the depth, and you can cut, for example, starting 20% of full depth, and then step up to 100%.






Title: Re: V-Engrave Plugin
Post by: Bubba on September 07, 2014, 14:23:24 pm
I like the angle adjustment for depth.  The issue I was struggling with for doing multiple passes was how to make a smooth final pass and avoid any steps.
===================
Would it possible to have a maximum depth option (selection) so user can simply measure the bit flute length and determine the depth of the cut? On deeper cuts in wood I don't see as a problem with minimal step. Something it can easily be dealt with. I have used your plugin couple times and job always come out as expected. Nicely done! Thanks.


Title: Re: V-Engrave Plugin
Post by: pstemari on September 07, 2014, 17:34:18 pm
It's there, but it's implied by the tool diameter.  The max depth is 1/2*(tool diameter - tool tip diameter)*cot(V-Angle / 2).

In other words, it won't ever plunge past the tool diameter. 


Title: Re: V-Engrave Plugin
Post by: Bubba on September 07, 2014, 19:02:57 pm
It's there, but it's implied by the tool diameter.
++++++++++++++++++

OK, I didn't know that. Thanks.


Title: Re: V-Engrave Plugin
Post by: elf on September 18, 2014, 19:16:53 pm
Attached are two .cb files. The first, L_Font.cb, is based on a TrueType font, the second, L_Inkscape.cb, on the same font converted to lines and arcs using Inkscape. 

V-Engrave appears to generate the correct toolpath in L_Font.cb but doesn't in L_Inkscape.cb.  What changes do I need to make for V-Engrave to generate the correct toolpath in L_Inkscape.cb?


Title: Re: V-Engrave Plugin
Post by: Bubba on September 18, 2014, 20:18:00 pm
convert it to 'region' first. It does work fine here.


Title: Re: V-Engrave Plugin
Post by: elf on September 20, 2014, 06:41:12 am
Thanks, that works.  Now to figure out what the settings will be for the inlay piece :)


Title: Re: V-Engrave Plugin
Post by: ajayre on September 21, 2014, 21:39:51 pm
I've tried cutting the outside of the letter 'C' and at one point the v-engrave path deviates from the curve of the letter. See the screenshot.

The problem isn't a display issue because CutViewer shows the same defect.

Any ideas on how to fix it?

Thanks, Andy


Title: Re: V-Engrave Plugin
Post by: ajayre on September 21, 2014, 21:44:52 pm
How can I get the VCarve Pro effect shown in this image?

(http://www.vectric.com/products/vcp/features/images/prism.jpg)

By using V-engrave on a region and the pocketing the region with a suitable roughing clearance the attached image is the closest that I have come, but this method leaves a plateau on top of the letter.

Thanks, Andy


Title: Re: V-Engrave Plugin
Post by: blowlamp on September 21, 2014, 23:33:44 pm
How can I get the VCarve Pro effect shown in this image?

(http://www.vectric.com/products/vcp/features/images/prism.jpg)

By using V-engrave on a region and the pocketing the region with a suitable roughing clearance the attached image is the closest that I have come, but this method leaves a plateau on top of the letter.

Thanks, Andy

I don't think you can use the current V-Engrave plugin to get this effect.

The Profile MOP does a fair job if you use a truncated cone cutter and run it around the outside of the character (Tool Diameter set to equal the truncated diameter), whilst specifying a Cut Depth large enough for the central ridge to form. This method doesn't give the sharp inner corners to certain letters (E, F, K, etc) that a dedicated Prism MOP would give, but it's still pretty good.


Martin.


Title: Re: V-Engrave Plugin
Post by: pixelmaker on September 22, 2014, 01:04:44 am
hello,
you can make this also with the v-engrave plugin.
You need the letter, you draw a second polyline with the offset function and a third polyline with the half of the distance of the first offset.
The letter and the first offset line you convert in to a region. After you use STR+U on this region.
To cut "inside" the letter you set the stock surface lower then the stock. As lower you set the stock as more you cut to the middle of the letter.
The second polyline with the half distance you need for the pocket.
In the attached file you see how I do this.
You need a cutter with a flat v-angle and a large diameter.

ralf


Title: Re: V-Engrave Plugin
Post by: elf on September 22, 2014, 02:51:58 am
hello,
you can make this also with the v-engrave plugin.
You need the letter, you draw a second polyline with the offset function and a third polyline with the half of the distance of the first offset.
The letter and the first offset line you convert in to a region. After you use STR+U on this region.
To cut "inside" the letter you set the stock surface lower then the stock. As lower you set the stock as more you cut to the middle of the letter.
The second polyline with the half distance you need for the pocket.
In the attached file you see how I do this.
You need a cutter with a flat v-angle and a large diameter.

ralf

The technique in the Inlay portion of this thread will also create raised letters with sharp crests: http://www.cambam.co.uk/forum/index.php?topic=4065.0


Title: Re: V-Engrave Plugin
Post by: ajayre on September 22, 2014, 21:28:00 pm
Thanks! I'll give those suggestions a try.

Andy


Title: Re: V-Engrave Plugin
Post by: ajayre on September 23, 2014, 09:51:09 am
Ralf,

Your technique worked well - see attached. Thanks!

Any ideas why the vengrave toolpath is executed three times?

Andy


Title: Re: V-Engrave Plugin
Post by: pixelmaker on September 23, 2014, 10:52:02 am
It looks that if you convert the two lines to a region the letter is cut two times and if you use the join (Strg+U) it cuts 3 times.
This is a problem of the engrave plugin, I am only a user and I can tell you only the workaround.
Create a new, active layer
Right Mouse on the mop and "toolpath to geometry"
Delete the v-engrave mop.
On the new layer are now two or three polylines for each sign. Delete the needless polylines and use a engraving mop to cut this polylines.

ralf


Title: Re: V-Engrave Plugin
Post by: CaesarS on December 18, 2014, 06:18:32 am
Hi there!

New to CamBam, I like it so got the license  :)

I've installed the plug in and able to select it in the Machining menu list.

I don't know how to use it though? On my test cut it promptly plunged into the depths to the point my stepper motors skipped steps.

I don't see a way to configure depth increments, how would I control the depth per pass?

Thanks, Caesar.


Title: Re: V-Engrave Plugin
Post by: EddyCurrent on December 18, 2014, 09:43:45 am
You don't control the depth specifically. You need a large enough V cutter for the particular job such that it 'fills' the character at a reasonable depth of cut.

Also read these two posts;
http://www.cambam.co.uk/forum/index.php?topic=3513.msg31263#msg31263


Title: Re: V-Engrave Plugin
Post by: Bubba on December 18, 2014, 13:12:06 pm
I don't know how to use it though? On my test cut it promptly plunged into the depths to the point my stepper motors skipped steps.
++++++++++++++++++++
Because the depth can not be controlled, I have used phony V tool diameter, usually a 1/3 bigger than the cutter I intent to use just to create a gcode. It worked for me fine..


Title: Re: V-Engrave Plugin
Post by: CaesarS on December 18, 2014, 15:06:02 pm
Aaaaah that makes sense now, I'll try it out.


Title: Re: V-Engrave Plugin
Post by: macbob on December 18, 2014, 15:34:22 pm
I found that if I gave a non-zero cutter diameter then I had to be careful that it did not exceed the Max Crossover Distance, since otherwise the path tended to traverse from one region to another without fully retracting to the clearance plane.  Check your rapids!

I would have thought that if the cutter is going too deep, it must imply that the width of the outline was root 2 times bigger than this?  I found it handy to draw myself a circle with diameter equal to the actual cutter size and to drag it round my drawing looking to ensure that it never fit entirely within the region.

Bob


Title: Re: V-Engrave Plugin
Post by: EddyCurrent on December 18, 2014, 16:49:47 pm
It just requires something to parse the generated G code file to find the extremes of Z


Title: Re: V-Engrave Plugin
Post by: lloydsp on December 18, 2014, 17:05:38 pm
It just requires something to parse the generated G code file to find the extremes of Z
-----------
You have that in CB, Eddy.

Import the g-code, then convert toolpaths to geometry.

Then just select it all, and get the object extremas.

LLoyd


Title: Re: V-Engrave Plugin
Post by: EddyCurrent on December 18, 2014, 17:29:50 pm
It just requires something to parse the generated G code file to find the extremes of Z
-----------
You have that in CB, Eddy.
LLoyd

Thanks, yes I tried that before I posted because it returned zero.
Obviously that was correct because I had not imported the g-code and implemented Toolpaths to Geometry.


Title: Re: V-Engrave Plugin
Post by: Dragonfly on December 18, 2014, 18:26:19 pm
I haven't tried the V-Engrave plugin but from what I read it definitely needs max depth limit. If the depth is not enough to fill a gap then a step over move should be added to cover for it. I've seen other programs work this way and when the area is relatively large they produce a flat bottom at that place.

Really have to see the plugin, my comments are somewhat random now.


Title: Re: V-Engrave Plugin
Post by: Bubba on December 18, 2014, 20:53:03 pm
If the depth is not enough to fill a gap then a step over move should be added to cover for it. I've seen other programs work this way and when the area is relatively large they produce a flat bottom at that place.
+++++++++++++++

The same here. It cetainly would help when v-carving thin material


Title: Re: V-Engrave Plugin
Post by: dh42 on April 07, 2015, 19:24:11 pm
Hello,

Maybe it's an already known problem (I don't use the plugin for my own usage) .. but on the last version (0.0.0.8 ) the cut width display don't work (I tried the 0.0.0.5 and it work)

++
David


Title: Re: V-Engrave Plugin
Post by: pstemari on April 22, 2015, 07:49:42 am
Sorry for the absence, been busy at work and working on some electronics projects.

I just moved the project over to GitHub from GoogleCode.  The new URL is https://github.com/pstemari/v-engrave-plugin.  I haven't integrated the patches in yet, just glad to get it moved before Google Code shuts down.

The problem with step-over moves is that getting a flat bottom when the cutter tip is 0.005" diameter would take forever.  Ideally you'd fill in a slight border and then come back with a square end mill to hog out the flat area.  For example, with the engraving cutters I use that would require ~20 loops around the perimeter with a 0.0017" step-over (D/3) to get a 0.0325" border and then switch to a 1/16" end mill to finish it up.


Title: Re: V-Engrave Plugin
Post by: EddyCurrent on April 22, 2015, 08:18:24 am
I was looking at your code for V engrave a while ago, it's very impressive and also a great plugin. Nice to see you back too.


Title: Re: V-Engrave Plugin
Post by: Dragonfly on April 22, 2015, 11:53:31 am
Quote
The problem with step-over moves is that getting a flat bottom when the cutter tip is 0.005" diameter would take forever.
That's not always true. There are V-cutters with flat tips of 0.5 to 1 or more mm width. Besides if it is an artistic type of engraving the author may choose to leave tool trails instead of a flat bottom.
Anyway I've seen this implemented in Vectric programs, they have included such tools and path approach. The trouble is - they cost a lot :)


Title: Re: V-Engrave Plugin
Post by: Bubba on April 22, 2015, 21:35:25 pm
Quote
The problem with step-over moves is that getting a flat bottom when the cutter tip is 0.005" diameter would take forever.
That's not always true. There are V-cutters with flat tips of 0.5 to 1 or more mm width. Besides if it is an artistic type of engraving the author may choose to leave tool trails instead of a flat bottom.
Anyway I've seen this implemented in Vectric programs, they have included such tools and path approach. The trouble is - they cost a lot :)

Exactly! :D


Title: Re: V-Engrave Plugin
Post by: pstemari on May 05, 2015, 23:22:58 pm
Yeah, I keep forgetting about router uses.

My stuff all uses the Precise Bits (http://www.precisebits.com/products/carbidebits/scoreengrave.asp) cutters from Soigeneris (http://www.soigeneris.com/engraving-list.aspx).


Title: Re: V-Engrave Plugin
Post by: Bubba on May 06, 2015, 12:42:37 pm
Most of the time I use the V60 Deg cutter by CMT Recently used it to carve with g code created by Artcam(available occasionally when visiting a friend) and it did not have any problem clean up .200" wide space with it. It took some time, but to be expected.. So..I can only wish for the V-carve plugin to work in similar fashion. To be able to control the depth of the cut, and the material be removed when needed even if it would take on minutes.. 

 http://www.cmtutensili.com/show_items.asp?pars=RB~7/8/958~2~2.


Title: Re: V-Engrave Plugin
Post by: RickinBeachcrest on May 09, 2015, 03:35:42 am
What is the latest version of V-engrave?  I have been using v7.

Also how do you set the default tool that will be used by V-engrave?

Thanks.
Rick



Title: Re: V-Engrave Plugin
Post by: EddyCurrent on May 09, 2015, 10:46:46 am
Generally the best place to look is here; http://www.cambam.co.uk/forum/index.php?topic=4269.msg30083#msg30083
It looks like V engrave is at version 8
There is no default tool as far as I'm aware, that has to be populated by youself like any other MOP unless you use a Template or CAM style.
All I did was create some tools in my Tools Library; http://www.cambam.info/doc/plus/cam/ToolLibrary.htm


e.g.

Name "0.00mm 2 flute V-Cutter 90.00 deg"
Diameter 12
Tool Number 17
Profile VCutter
Tip Diameter  0
Angle 90



Title: Re: V-Engrave Plugin
Post by: dh42 on January 24, 2016, 21:18:59 pm
Hello,

I just remark a problem in the last version of the V-engrave plugin that is not in the B0004 version.(the last version from Pstemari I think) It appears in the B0006 and it is also present in B0008.

Try with the simple file in attachment ; with the B0004 (link on the first message) all is OK, but with the last B0008 or B0006 the toolpath are created twice. (and also the cutwidth display don't work)

You can easily see that by converting toolpath to geometries ; all exists twice.

Lloyd, if I well remember you work on the plugin since B0006 ; The duplicate TP are a "features" you adds or a bug ?

Another pb (on all version) is that if we rotate a text, the toolpath are wrong for the chars that contain a region ; need to explode the text first.

++
David


Title: Re: V-Engrave Plugin
Post by: lloydsp on January 24, 2016, 22:30:48 pm
David,
I do not remember.  I'm on a client's site right now, so I cannot spend too much time on other that a few web-checks and emails.

I'll try to look later in the week, if you don't find 'hard evidence' before then.

LLoyd


Title: Re: V-Engrave Plugin
Post by: dh42 on January 24, 2016, 22:36:28 pm
Quote
I'll try to look later in the week, if you don't find 'hard evidence' before then.

Hello Lloyd,

I take a look on the source (the last available are 0006), but .... I understand nothing ... C# is not for me  :-[

Quote
I cannot spend too much time on other that a few web-checks and emails

There is no emergency ;)

++
David


Title: Re: V-Engrave Plugin
Post by: lloydsp on January 24, 2016, 22:44:59 pm
'Found it pretty quickly.  I added ONE line to continue the segment loop if a segment was too short, or the turn angle was zero.

" On 3/10/14, MacBob found another one.  When Paul processed a segment too short to do any math
 upon, he issued a warning message, but didn't skip that segment.  As a result, he ended up
 with an N/A value in the structure "dse" down in the FollowOutline routine.  Look for the "OOPs!" in
 FollowOutline in Plugin.cs (this file).
 */

And this in the "FollowOutline" procedure:  just search for the "If (len < DBL_EPSILON)", which is unique in this file.

      if (len < DBL_EPSILON) {         
           // the Warning message changed 3/10/14 to something meaningful.  LES
           //_log.Log(WARNING, "Primitive {0}[{1}] is too short.", outline.ID, i);
           // message level is changed so the user doesn't usually see it, since it refers to internal operations
           
          _log.Log(DEBUG, "Primitive {0}[{1}] is too short to cut, so it is being skipped.", outline.ID, i);

          //  OOPs! Paul didn't skip it!!... if it's zero length or too short to process,
          // then it's ALSO too short to mill... SKIP the segment instead of just issuing warnings!
          // Failure to skip the segment almost guarantees a math error or undefined result.  LES 03/10/14
 
//  Add this code change to skip the segment ---
           continue;   // don't abandon the whole outline, just this one segment -- added 3/10/14 LES
 //  End modification 3/10/14

         }


Title: Re: V-Engrave Plugin
Post by: dh42 on January 24, 2016, 22:54:11 pm
Sorry Lloyd, I don't understand  :-[ ... it's a bug or it's needed that all the toolpath always exists twice ?

++
David


Title: Re: V-Engrave Plugin
Post by: lloydsp on January 24, 2016, 23:58:32 pm
The simple bug was that if a line was too short to calculate, or if the arc radius between two segments was zero, it would cause a math exception.  The 'continue' I added simply allows that one segment or arc to be skipped as if it did not exist.

It has nothing to do with coursing the lines twice.  I never looked for or addressed that issue -- didn't even know it was a problem!

Lloyd


Title: Re: V-Engrave Plugin
Post by: dh42 on January 25, 2016, 15:25:37 pm
Quote
It has nothing to do with coursing the lines twice.  I never looked for or addressed that issue -- didn't even know it was a problem!

I have used the plugin only one time for "real" job ; On the simulator, it's difficult to see that the toolpath exists twice because it do the job quickly ... but on the real machine It's obvious ..

Also since the B0006, the ShowCutwidth no longer work.

++
David


Title: Re: V-Engrave Plugin
Post by: cyberwollf on June 05, 2016, 02:05:47 am
Are the older versions located anywhere?  I downloaded the b008 (but the "About VEngrave" only shows b007) and it cut everything multiple times.  Was there ever a workaround for this or a link to an older working version?


Title: Re: V-Engrave Plugin
Post by: dh42 on June 05, 2016, 17:49:02 pm
Hello,

The B0004 can be downloaded here
http://v-engrave-plugin.storage.googleapis.com/v-engrave-plugin-latest.zip

It's the last version without the bug that cut all twice and also the last that show the cutwidth

++
David


Title: Re: V-Engrave Plugin
Post by: cyberwollf on June 05, 2016, 20:57:29 pm
Hello,

The B0004 can be downloaded here
http://v-engrave-plugin.storage.googleapis.com/v-engrave-plugin-latest.zip

It's the last version without the bug that cut all twice and also the last that show the cutwidth

++
David

Any downside to using this version over b008?  Known issues/limitations with b004?


Title: Re: V-Engrave Plugin
Post by: dh42 on June 05, 2016, 21:13:22 pm
some pb with circle ; you can read more here about bug removed since the 0004, (but unfortunately, other added  :( )

http://www.cambam.co.uk/forum/index.php?topic=3513.45

I use very rarely the V-engrave plugin, but for my use, I've replaced the 0008 by the 0004 because the twice cut pb.

++
David


Title: Re: V-Engrave Plugin
Post by: cyberwollf on June 05, 2016, 22:05:11 pm
some pb with circle ; you can read more here about bug removed since the 0004, (but unfortunately, other added  :( )

http://www.cambam.co.uk/forum/index.php?topic=3513.45

I use very rarely the V-engrave plugin, but for my use, I've replaced the 0008 by the 0004 because the twice cut pb.

++
David

Thanks!  I'm looking to try some inlay work. Would you recommend f-engrave over the vcarve plugin?


Title: Re: V-Engrave Plugin
Post by: EddyCurrent on June 05, 2016, 22:15:41 pm
Did you see this ? http://www.atelier-des-fougeres.fr/Cambam/Aide/Plugins/InlayCalculator.html


Title: Re: V-Engrave Plugin
Post by: dh42 on June 05, 2016, 22:15:58 pm
Quote
Would you recommend f-engrave over the vcarve plugin?
I don't know F-engrave.


Title: Re: V-Engrave Plugin
Post by: EddyCurrent on June 05, 2016, 22:17:05 pm
here; http://www.scorchworks.com/Fengrave/fengrave.html
Scorch has some great software.


Title: Re: V-Engrave Plugin
Post by: cyberwollf on June 05, 2016, 23:01:20 pm
I Finally got some light and dark stock to try inlay.  I have the calculator plugin and everything figured out, just wanted to make sure I had the "best" version of the plugin before I make the cuts.


Title: Re: V-Engrave Plugin
Post by: cyberwollf on June 07, 2016, 13:39:02 pm
Hello,

The B0004 can be downloaded here
http://v-engrave-plugin.storage.googleapis.com/v-engrave-plugin-latest.zip

It's the last version without the bug that cut all twice and also the last that show the cutwidth

++
David

There is no DLL file here.  Do you have a link for how to install?


Title: Re: V-Engrave Plugin
Post by: EddyCurrent on June 07, 2016, 14:12:56 pm
I just tried the link and it works for me.
Download the zip file then unzip it to reveal the dll
Move the dll file to CamBam's 'Plugins' folder
Restart CamBam


Title: Re: V-Engrave Plugin
Post by: EddyCurrent on September 09, 2016, 20:19:10 pm
I just uploaded b0005.  Nothing major, some fixes for the z-position at the beginning and end of each cut. . . .

David,

This is why the 'Show Cut Widths' stopped working, Lloyd is innocent  :D


Title: Re: V-Engrave Plugin
Post by: dh42 on September 09, 2016, 20:40:51 pm
Hello Eddy

apologies to Lloyd  ;D Tonight I would be deprived of dessert  :'(

The fact that the 'Show Cut Widths' stopped working is not really a pb, but the fact that all toolpath exists twice increase machining time x2 .. I have not see that until I really cut something with the CNc and not only the CV simulator (I used it only one time for real, on the "cat house" ;)) and when I convert toolpath to geometries to try to understand why the machine cuts two pass I see that there is two identical toolpath superimposed)

your are working on the plugin ? A new multipass version  ? ;D ;D

++
David


Title: Re: V-Engrave Plugin
Post by: EddyCurrent on September 09, 2016, 20:53:49 pm
David,

The same changes that pstemari made for version b0005 are also the reason for the cuts occuring twice.
It's quite complex code so even though I know where the problems exist I've not got to the point of a solution.





Title: Re: V-Engrave Plugin
Post by: dh42 on September 09, 2016, 20:58:46 pm
Quote
It's quite complex code

I agree ! .. I have a look on it when I fall on the TP problem ... but I understand nothing  :-[ too complex for a noob as me (and C is not my "natural" language)

++
David


Title: Re: V-Engrave Plugin
Post by: Bubba on September 09, 2016, 21:34:47 pm
but the fact that all toolpath exists twice increase machining time x2
*********************
Personally, I think it the code is created to cut in climb mode and come back with conventional. It seems to me that it does purposely. Al least it appears that way to me. It was while back when I used ..  But, I do like it, because it does cleanup the remaining burr to the point that after cut very little if any hand work is necessary. Now if somebody is in production mode and machine time is closely observed then it maybe an issue. The only thing I would like changed is to be able to control the maximum depth of cut instead of infinite as is now. Because in some cases is not really practical..

My 2¢


Title: Re: V-Engrave Plugin
Post by: EddyCurrent on September 09, 2016, 21:50:28 pm
It looks like the same line of code was written twice in error, I 've deleted one of the lines and the code does not run twice now.
I'm now working through the changes Lloyd made and should end up with a good version.

However,. time for bed here  ;)


Title: Re: V-Engrave Plugin
Post by: dh42 on September 09, 2016, 22:17:15 pm
Hello

Quote
I 've deleted one of the lines and the code does not run twice now.

Hurrah !! you are the king ;)

Good night
++
David


Title: Re: V-Engrave Plugin
Post by: Bubba on September 10, 2016, 00:22:46 am
Here is the latest work I did using V-engrave plugin v.0007 along with Inlay Calculator plugin. All did great. The woods used is Walnut and Maple..


Title: Re: V-Engrave Plugin
Post by: pstemari on September 10, 2016, 02:14:10 am
Not certain if I've explained this before, but the reason you'll see it cutting the same path twice in opposite directions is that it's working around the perimeter of the font outline. So, for something like an L, it will go up the left side of the stem, across the end, down the right side, across the top of the foot, down the end, and finally back along the base of the foot.  As it goes, it's calculating how far over and down it needs to go to touch the opposite side. The result is that the naive calculation will cut though each point, once for each side.

At one point I believe I added code to attempt to avoid that, but how well it works I don't recall. At any rate, it's doing what amounts to a plunge slotting operation, which is climb cutting on one side and conventional cutting on the other side.



Title: Re: V-Engrave Plugin
Post by: Bubba on September 10, 2016, 02:59:04 am
Not certain if I've explained this before, but the reason you'll see it cutting the same path twice in opposite directions is that it's working around the perimeter of the font outline. So, for something like an L, it will go up the left side of the stem, across the end, down the right side, across the top of the foot, down the end, and finally back along the base of the foot.  As it goes, it's calculating how far over and down it needs to go to touch the opposite side. The result is that the naive calculation will cut though each point, once for each side.

At one point I believe I added code to attempt to avoid that, but how well it works I don't recall. At any rate, it's doing what amounts to a plunge slotting operation, which is climb cutting on one side and conventional cutting on the other side.


Thanks for explaining this. I like how this plugin perform. ;)


Title: Re: V-Engrave Plugin
Post by: EddyCurrent on September 10, 2016, 14:36:27 pm
After watching the toolpath while manualy stepping through in CutViewer, I'm fairly confident the tool is following a path described above by pstemari, but only once.
I have also disabled the messages and the speed increase in gcode generation is huge.

Hope to have a test version later today. :D



Title: Re: V-Engrave Plugin
Post by: dh42 on September 10, 2016, 15:05:58 pm
Hello,

Quote
I have also disabled the messages and the speed increase in gcode generation is huge.

Interesting to know ; by 'disabled', you want say 'switched to comments' in the code or you use a higher diag level in the message function (and a lower in the options to shut down the display)

++
David



Title: Re: V-Engrave Plugin
Post by: EddyCurrent on September 10, 2016, 18:31:30 pm
Hello,

Quote
I have also disabled the messages and the speed increase in gcode generation is huge.

Interesting to know ; by 'disabled', you want say 'switched to comments' in the code or you use a higher diag level in the message function (and a lower in the options to shut down the display)

++
David


David,
I just commented out the lines that print the messages.

Please try the attached version b0009

* 'Show Cut widths' works
* lines only cut once instead of twice
* all changes by Lloyd added
* messages disabled to speed things up (plan to make this user selectable later)

David's test file is also attached (text slightly changed to include an 'L' to test as pstemari described.



Title: Re: V-Engrave Plugin
Post by: dh42 on September 10, 2016, 20:04:50 pm
Hello,

I'll try it tomorrow  ;)

Quote
plan to make this user selectable later

You can just use a value like 4 for DiagnosticLevel, so the texts appears in the log message only if the diag level is set to 4 or more in the general options.

static void AddLogMessage(int DiagnosticLevel, string msg)

++
David


Title: Re: V-Engrave Plugin
Post by: tau on September 10, 2016, 20:18:31 pm
Hi Everyone!

Nice to see that Plugin-Dev Team is still alive!  ;D

@Eddy

Even though i haven't really use the V-Engrave Plugin, i just fired up CamBam with your newly provided version and the test file.

I was suprised to see some 'linear' segments in the engraving path of the 'O' letter. Most of the 'O' has a curved path which is what i expect to see, but why is this area linear?!

Is this just some minor bug in path calculation?

tunc


Title: Re: V-Engrave Plugin
Post by: EddyCurrent on September 10, 2016, 21:03:40 pm
David,

Okay, I'll give that a try but I'm away for a few days now and computer free  ;D

tunc,

Thank you for testing this.

I tried David's test file using version b0004 of the plugin and it behaves in exactly the same way, so it's not something I have introduced.

The short answer is, I don't think I'm in a position to sort out any bugs of that nature, the reason being that I don't have a full comprehension of the code.

My goal was just to fix some things that had gone wrong along the way.


Title: Re: V-Engrave Plugin
Post by: dh42 on September 11, 2016, 18:26:44 pm
Hello,

Nice job Eddy  ;D

Quote
I tried David's test file using version b0004 of the plugin and it behaves in exactly the same way, so it's not something I have introduced.

Yes, it's an old problem that appears sometimes on circular shapes. A way to solve it is to use a 'remove arcs' on the shape.

on the picture:

left side, a 'O' (arial) 100 mm height used as is.

right side, the same but -> convert to polyline (CTRL P) -> remove arcs 0.05 -> convert to region (CTRL I)

On thing that would be fine, if it is possible to do, is that the 'tool angle' in the plugin reflect the tool angle of the selected tool in the tool library ; if I select a 60° tool in the tool number list, the 'tool angle' in the plugin always show 90°

++
David


Title: Re: V-Engrave Plugin
Post by: pixelmaker on September 11, 2016, 21:19:55 pm
Thank you very much Eddy that the plugin now works with developer versions and it is really fast now.
(http://pixelmaker.eu/cambam/icon/daumen_hoch.gif)

ralf

@David

If you get this problems with letters or text then convert it to polyline and add points. In the attached file can you see this.


Title: Re: V-Engrave Plugin
Post by: dh42 on September 11, 2016, 21:51:58 pm
Hello Ralf

For me, not working on dev version ; I can create a V engrave mop and generate toolpath and Gcode, but I can't save it or open a file that use a Vengrave mop.

Maybe it need to be compiled for framework 4.0 (new cambam use it instead of 3.5)

++
David


Title: Re: V-Engrave Plugin
Post by: pixelmaker on September 12, 2016, 10:32:35 am
Yes David I see this after writing this answer.
Quote
Maybe it need to be compiled for framework 4.0
Is it possible to compile it for .NET 4 and .NET 3.5 ? Then we can work with P version and also with the dev version.
If I look for this error"there was an error reflecting type"  I get "XML Serialization issue"  and "Error reflecting type in XML generation".
This looks not like a .NET error


I work with the dev version  more and more. I work often with the splines.


ralf


Title: Re: V-Engrave Plugin
Post by: dh42 on September 12, 2016, 14:14:19 pm
Hello,

Hum, yes you are certainly right about the error.

Quote
I work often with the splines.

Yes, it's a nice new features 8)

++
David


Title: Re: V-Engrave Plugin
Post by: dh42 on September 12, 2016, 14:47:53 pm
Re

I just see that on dev version, if the V-engrave is installed we can't load/save anything ; not only files that use v-engave.

I think it's an improper way to add a new machining operation to CB file in the V-engrave plugin, because if I uses a thread mop in the alpha version, it is recognised, loaded/saved  and it's also a plugin that adds a new kind of mop. (but it cause very strange things in CB with toolpath display)

++
David



Title: Re: V-Engrave Plugin
Post by: EddyCurrent on September 13, 2016, 21:21:34 pm
Thanks for the testing and comments, now I'm fully refreshed from a mini break I'll have a play about to see what can be done.

Question - Is the dev version mature enough to start reworking plugins ?


Title: Re: V-Engrave Plugin
Post by: dh42 on September 13, 2016, 22:31:22 pm
Hello,

Quote
Question - Is the dev version mature enough to start reworking plugins ?

I think it is better to wait a little until the beta version is available, otherwise it may be work for nothing ; for now the dev version is only an alpha version; a lot of things can change until the beta version is ready.

++
David


Title: Re: V-Engrave Plugin
Post by: EddyCurrent on September 21, 2016, 17:06:59 pm
Please find version b0010 attached.

1. The 'About' box (Plugins->V-Engrave About) is now a form with a checkbox to enable/disable log trace messages.
    It defaults to messages disabled.

Hello,

On thing that would be fine, if it is possible to do, is that the 'tool angle' in the plugin reflect the tool angle of the selected tool in the tool library ; if I select a 60° tool in the tool number list, the 'tool angle' in the plugin always show 90°

++
David

Done

2. When a 'Tool Number' is selected, it's Vee Angle will automatically be inserted into 'Tool V-Angle'.
   If a tool is selected that does not have the Vee Angle parameter populated then 'Tool V-Angle' will go the the default value of 90.  


Title: Re: V-Engrave Plugin
Post by: dh42 on September 25, 2016, 22:02:41 pm
Hello,

Nice, seems to work well  ;)

++
David


Title: Re: V-Engrave Plugin
Post by: Bubba on December 15, 2016, 17:10:08 pm
It look like "Resident guru's" will be needed to recompile Vengrave plugin for the new CB version..
CB v1 complains.. Please see attachment.


Title: Re: V-Engrave Plugin
Post by: lloydsp on December 15, 2016, 17:26:01 pm
Andy made the point that plugins will have to be re-compiled.

Lloyd


Title: Re: V-Engrave Plugin
Post by: dh42 on December 15, 2016, 17:31:55 pm
Hello,

Yes, maybe just need to be recompiled with new dll and .net 4.0 (I hope for Eddy  :D :D)

there is a lot of other plugins that no longer works on V1.0 (or not totally works), like zoom toolbar, polygon ..

++
David


Title: Re: V-Engrave Plugin
Post by: lloydsp on December 15, 2016, 17:44:39 pm
"there is a lot of other plugins that no longer works on V1.0 (or not totally works), like zoom toolbar, polygon ..."
----
And others that have been rendered completely superfluous, like "print"!  :D

Lloyd


Title: Re: V-Engrave Plugin
Post by: Bubba on December 15, 2016, 17:49:24 pm
Agree,
I got this in yesterdays email from Andy.

"I forgot to put on the release email, that most plugins will need to be recompiled for the new release."

That's why I alerted 'Local Gurus' to aware of this.. ;D ;D

David, tested the 'Numerical Move' and 'Chamfer/Radius' plugins. Both seem to be working fine.

Was hoping the 'Dashed line plugin' created by Eddy would come to live.. No Joy.. :'(  


Title: Re: V-Engrave Plugin
Post by: Bubba on December 15, 2016, 17:55:21 pm
"there is a lot of other plugins that no longer works on V1.0 (or not totally works), like zoom toolbar, polygon ..."
----
And others that have been rendered completely superfluous, like "print"!  :D

Lloyd

Lloyd, But it served me and others well..
I still have plans for CB 9.8v, as long as lots of plugins won't work in new version CB.. So I may use the print plugin
thinking of man who created it..  ;D :-[ :'(, nah.. ;D ;D :D ;) 


Title: Re: V-Engrave Plugin
Post by: dh42 on December 15, 2016, 18:09:00 pm
Quote
Was hoping the 'Dashed line plugin' created by Eddy would come to live.. No Joy..

Lol, it's one of the first I test on V1.0  with no luck too.

Quote
David, tested the 'Numerical Move' and 'Chamfer/Radius' plugins. Both seem to be working fine.

For an unknown reason, it seems that all my plugins  are working on 1.0 (except 'arc center', but it's just a pb of menu item position and I can solve that easily)

I've an new idea to do dashed lines, but I want to finish the plugin I'm working on at the moment before to explore another way ..

Quote
I still have plans for CB 9.8v, as long as lots of plugins won't work in new version CB.. So I may use the print plugin

You can also swap from v0.9.8 to v1.0 depending of the job to do, so you can draw a spline on the 1.0, or digitize a picture (and transform to polylines) the copy/paste the objects to the 0.9.8 to do other job.

currently, I do not use the alpha version only, not because plugin pb, but because VBscript is not implemented and also because it has bug with copy/paste format.(2 things that I use a lot)

++
David


Title: Re: V-Engrave Plugin
Post by: Bubba on December 15, 2016, 19:13:01 pm
Yep, Thanks for that David. I'm staying with 9.8 mainly because of the VEngrave plugin. I got few jobs that require the plugin to work right. One is the Inlay using V-Engrave plugin calculator  I got a couple of jobs lined for that and couple of signs, So, I use the VEngrave plugin quite bit.

I appreciate your effort toward the dashed lines plugin. There been couple of times where It would make life easier..


Title: Re: V-Engrave Plugin
Post by: EddyCurrent on December 15, 2016, 19:32:17 pm
V-Engrave still won't work but neither does Threadmill and Trochoidal Pocket.
All those work by adding a new type of MOP so there is something common there.


Title: Re: V-Engrave Plugin
Post by: dh42 on December 15, 2016, 19:41:42 pm
Strange, trocho pocket works as a charm on the V1.0 for me  ??? ??? and also Threadmill .. except that on V1.0 the toolpath are missing on the display for Threadmill  (but the gcode is ok)

and ... no pb to use the same file with 0.98 and v1.0 ...

++
David





Title: Re: V-Engrave Plugin
Post by: dh42 on December 15, 2016, 22:29:24 pm
tried to recompile Vengrave with some debug text to find what is going wrong.

the error seems to appears at this line (in AttachToUI)

new XmlSerializer(typeof(MOPVEngrave)).Serialize(new MemoryStream(), new MOPVEngrave());

but ... I do not understand what is it and what it do .. ???

++
David


Title: Re: V-Engrave Plugin
Post by: EddyCurrent on December 15, 2016, 22:33:45 pm
This is the error message.
Other plugins work okay.


Title: Re: V-Engrave Plugin
Post by: EddyCurrent on December 15, 2016, 22:36:34 pm
 if (CADFile.ExtraTypes == null)  { CADFile.ExtraTypes = new List<Type>(); }
 CADFile.ExtraTypes.Add(typeof(MOPVEngrave));

  // HACK: Per 10bulls, this fixes clipboard errors associated with
 // copying external assembly objects that have not been serialized.

 new XmlSerializer(typeof(MOPVEngrave)).Serialize(new MemoryStream(), new MOPVEngrave());


Title: Re: V-Engrave Plugin
Post by: dh42 on December 15, 2016, 23:05:39 pm
wait a minute, I found the pb and it seems to works !  8) 8)


Title: Re: V-Engrave Plugin
Post by: dh42 on December 15, 2016, 23:31:43 pm
Ok, V engrave repaired, now it works on both 0.9.8 and and V1.0  8)

http://www.atelier-des-fougeres.fr/Cambam/Aide/Plugins/Vengrave.html

@ Eddy:

recompiled with .net 3.5 as usual (and of course .98 dll)

I only replace a statement and it works !

in plugin.cs

 close to line 230

[XmlType("MOPVEngrave"), Serializable]

is fully replaced by

[Serializable]

Code:
              foreach (TreeNode opNode in partNode.Nodes)
                {
                    if (opNode.Tag == mop)
                    {
                        mop.Name = opNode.Text;
                        opNode.EnsureVisible();
                        break;
                        }
                    }
                    break;
             }
        }

        foreach (var smop in CamBamUI.MainUI.CADFileTree.SelectedMOPs)
        {
            ThisApplication.AddLogMessage("SelectedMOPs: {0}", smop.Name);
        }
    }
    }

    //[XmlType("MOPVEngrave"), Serializable]
    // dh42: changed with [Serializable] so it works with V1.0

    [Serializable]
    public class MOPVEngrave : MOPFromGeometry, IIcon
    {
    // Smallest number such that 1.0 + DBL_EPSILON != 1.0
    const double DBL_EPSILON = 2.2204460492503131e-016;
    // Radians per degree
    const double DEGREES = Math.PI/180.0;
    // Log levels
    const int ERROR = 0, WARNING = 1, INFO = 2, DEBUG = 3, TRACE = 4, FINE = 5, FINER = 6, FINEST = 7;
    // logger

maybe something to test with dashed line plugin  ;D ;D (Makes a prayer !)

you know what ? I'm happy  :D

++
David


Title: Re: V-Engrave Plugin
Post by: dh42 on December 16, 2016, 00:09:04 am
it's me again  ;D

I've a try with dotpolyline with replacing [XmlType .... ] by [Serializable] no change ...

on 0.9.8, error when loading plugin, and error when saving the file

on 1.0, no error when loading the plugin or saving the file, but error "UnKnow entity type: DotPolyline" when loading.

 :-[ :-[

good night
++
David


Title: Re: V-Engrave Plugin
Post by: Bubba on December 16, 2016, 02:36:32 am
As Always, an awesome job David. The VEngrave plugin working like a champ in CB V1. Much appreciated. Thanks.
   


Title: Re: V-Engrave Plugin
Post by: EddyCurrent on January 08, 2017, 11:05:20 am
New version 12 attached

1. compiled with .NET 4
2. works with CamBam version 1 only
3. works in Windows and Linux

Thanks to David for the [Serializable] fix  ;D


Title: Re: V-Engrave Plugin
Post by: michel on January 09, 2017, 15:19:40 pm
Hi,

I tried the plug in and it works very well . However I have 2 issues


I cannot setup camotics to run the simulation with a v-cutter . It seems to only use round shapes even if i try to change it in camotics directly


second issue is that this is taking a lot fo memory . How can I reduce the g-code and still keep a decent result ?
my cnc memory is limited to 31.5 K . For stairs more then enough but not for such issues and it happens that I need it for a project .

I can manage it with the engrave plug-in and this one already pushing the limit of the memory. I just want to try to see if the v-engrave gives a better result.


regards
Michel


Title: Re: V-Engrave Plugin
Post by: dh42 on January 09, 2017, 19:20:17 pm
Hello,

Quote
second issue is that this is taking a lot fo memory . How can I reduce the g-code and still keep a decent result ?

Maybe you can play with Path Step Size to reduce the number of Gcode line .. if you increase this value, you get few lines in the toolpath.

++
David


Title: Re: V-Engrave Plugin
Post by: kitwn on March 06, 2017, 05:16:06 am
I was starting to think I would need to spend$460AUD on V-Carve to be able to produce the text carvings I want to make. That's a lot of money for something that is just a hobby.
Then a second round of CamBam related searching took me to the 'atelier-des-fougeres' website and there I found the goldmine!

Not just V-Engrave, which works perfectly with my DIY, LinuxCNC driven router, but a whole host of other really useful plugins. A very big THANKYOU! to everyone who's efforts make CamBam even better than it already is.

Kit


Title: Re: V-Engrave Plugin
Post by: dh42 on March 06, 2017, 22:47:59 pm
Hello

Welcome to the forum ;)

++
David


Title: Re: V-Engrave Plugin
Post by: kitwn on March 07, 2017, 06:04:41 am
Thankyou David,

I've been using CamBam for various simple jobs for a couple of years now but haven't paid much attention to the forum until very recently. It has certainly paid off in the last few days.

Regards

Kit


Title: Re: V-Engrave Plugin
Post by: lloydsp on March 07, 2017, 12:35:13 pm
Kit,
I won't chide you for not participating, but I think (as you've begun to discover) that this forum is part of the value of CamBam.

We have a lot of VERY GOOD and knowledgeable contributors here, who selflessly give of their time to help.  And, FWIW, help nearly always comes FAST.  I've frequently been the beneficiary of it.

LLoyd


Title: Re: V-Engrave Plugin
Post by: kitwn on May 28, 2017, 06:50:17 am
Lloyd,
I am gratefully un-chided  ;D

Just when I get to the point of being able to do the text carving I want I manage to terminally overheat the Makita router I was using as a spindle. Not the machine's fault I hasten to add, I had it mounted in a very poorly ventilated space on a very hot day.

Anyway here I am back in action again and just wanted to highlight the solution to a problem which David briefly pointed out on the forum last year but which had me confused for a while...

Text which contains a closed region (letters like A, a, B, b etc) will not produce correct tool paths after being rotated. The contained region is ignored and the letters will be engraved according to the outside of the letter shape only.
David said the letters need to be 'exploded' to overcome this. I found that selecting the text and then selecting 'Edit', 'Convert To', 'Region' (Ctrl + I is the shortcut for this) will overcome the problem. Each letter gets converted to a region and then carves as normal.

Kit


Title: Re: V-Engrave Plugin
Post by: lloydsp on May 28, 2017, 20:23:43 pm
Kit,
Thank you!  YOU just contributed to the group's knowledge!

Lloyd


Title: Re: V-Engrave Plugin
Post by: dh42 on July 07, 2017, 17:24:07 pm
Hello

I just see that with CB 1.0 R13 and the V engrave plugin V 0.0.1.1 or 0.0.1.2 the copy/paste and copy/paste format for the V-engrave Mops is not working.

"unable to find 'Vengrave plugin...' assembly"

++
David


Title: Re: V-Engrave Plugin
Post by: Bubba on November 07, 2017, 21:07:05 pm
Hello

I just see that with CB 1.0 R13 and the V engrave plugin V 0.0.1.1 or 0.0.1.2 the copy/paste and copy/paste format for the V-engrave Mops is not working.

"unable to find 'Vengrave plugin...' assembly"

++
David

Run into the same problem . V-engrave MOP plugin can not be copy/>paste format< the same way other MOP's are. Any Suggestions.
CB 1 R13...


Title: Re: V-Engrave Plugin
Post by: dh42 on November 08, 2017, 00:52:25 am
Hello

No, It works with 0.98 (V0011) but both V0011 and V0012 doesn't works for copy/paste on CB V1.0

I assume something has changed in CB V1.0 and that the plugin must be adapted.

++
David



Title: Re: V-Engrave Plugin
Post by: Bubba on November 08, 2017, 01:49:49 am
 doesn't works for copy/paste on CB V1.0
*************
That's what I meant and said.  I use CB v1.0 r13


Title: Re: V-Engrave Plugin
Post by: MX4000 on January 04, 2018, 10:39:50 am
Hi,

i have a problem with the v-engrave plugin when the V-Tool moves from an finished contour/letter to the next one. The problem is that the tool does not use allways the safety height from the properties in V-Engavre-MOP. Then the carver moves directly on the survace on Z=0.0 to the next contour. But sometimes the Surface isn't perfect even and it mills in this time in the workpiece. Is ther any adjustment to prevent this problem?
Thanks in advance :)
Martin


Title: Re: V-Engrave Plugin
Post by: lloydsp on January 04, 2018, 11:53:21 am
Set your 'max crossover distance' in the engrave MOp to zero. 

Some guys just leave make it zero as their style default, so they never have to check it unless they WANT no-lift crossovers between elements.

Lloyd


Title: Re: V-Engrave Plugin
Post by: MX4000 on January 04, 2018, 12:13:13 pm
Hi Lloyd,
This is the solution, it works.
Many Many Thanks!!  :D

Martin


Title: Re: V-Engrave Plugin
Post by: Dragonfly on January 04, 2018, 14:02:49 pm
Perhaps it also depends on whether you have set the shank diameter or the tip width as the tool diameter in the tools table. Or maybe the plugin uses the wrong tool property. I've never used it.


Title: Re: V-Engrave Plugin
Post by: Mark81 on August 27, 2018, 12:09:03 pm
I hope it's correct to append a message related to this plugin here instead of opening a new thread. If I'm wrong please tell me and I will start a new one. In some other forums is mandatory to continue the original thread, I don't know here  ::)

The documentation of the plugin (http://www.atelier-des-fougeres.fr/Cambam/Aide/Plugins/Vengrave_doc_EN.html (http://www.atelier-des-fougeres.fr/Cambam/Aide/Plugins/Vengrave_doc_EN.html)) says:

Quote
This plugin does not support multiple passes for the moment, so you should be careful. In case it is not possible to take all the depth of a sudden, you can limit the maximum depth with the Max Depth property, and use several separate operations.

Let's suppose I have a 6 mm 60° V-cutter and I want to limit the passes to 1 mm, where the actual maximum depth is 3 mm. I'm not sure to understand how to setup the next operations. I have to set the max depth of the first one to 1 mm, then it's enough to set the following to 2 and 3 mm? Or I also need to change the stock surface to -1 and -2?


Title: Re: V-Engrave Plugin
Post by: EddyCurrent on August 27, 2018, 12:46:49 pm
Make three VEngrave MOPs

the first one should have, Max Depth = 1
the second one should have, Max Depth = 2
the third one should have, Max Depth = 3

Everything else remains the same.


Title: Re: V-Engrave Plugin
Post by: EddyCurrent on August 30, 2018, 11:11:33 am
Thanks to JK, the master of serialization, we now have a version for CamBam v1.0 where copy and paste works with the MOp.  ;D

New version attached 12.01 for CamBam 1.0 only

1. Copy and paste works for MOps


Title: Re: V-Engrave Plugin
Post by: jk on August 30, 2018, 12:58:11 pm
Thats a title !


Title: Re: V-Engrave Plugin
Post by: kitwn on April 10, 2019, 04:39:37 am
I've just wasted far too much time wondering why V-engrave has suddenly stopped working correctly on my desktop PC. The symptoms were that CamBam carried on 'thinking' indefinately when calculating tool paths if I selected 22.5 degrees as my V angle. The default 90 was fine. I eventually realised that any integer angle was OK but the added .5 caused all the trouble.

The only change I could think of was that I'd recently changed my default postprocessor from 'default' which is what it has been for all the years I've used CamBam to 'LunuxCNC' which is what has driven my router without any trouble for just as long. It seemed like a good idea at the time! Changing it back again solved the problem.

Computers *!?*^%$!!!

Kit


Title: Re: V-Engrave Plugin
Post by: Bob La Londe on July 07, 2019, 17:05:10 pm
Set your 'max crossover distance' in the engrave MOp to zero. 

Some guys just leave make it zero as their style default, so they never have to check it unless they WANT no-lift crossovers between elements.

Lloyd


Its also an issue with some types of machining including basic text engraving.  Many of my finish styles have max crossover set to zero for this reason. 


Title: Re: V-Engrave Plugin
Post by: Bob La Londe on July 07, 2019, 17:28:21 pm
I am trying to determine some basic guidelines for using the V-Engrave plugin.  For example what tool diameter to use since the diameter varies based on the depth, and the depth should vary based on the space between the lines.  Do you go with tip diameter or shank diameter?  Also, does the V-engrave plugin account for tip diameter or assume V bits are perfectly pointed (which almost none are)?  My plan is to use a 60 degree spot drill with a 1/2" shank. 


Title: Re: V-Engrave Plugin
Post by: EddyCurrent on July 07, 2019, 17:41:33 pm
These are the settings I use for a 60 degree tool, it works well.
The comment is constructed to work with CutViewer simulator.
This is the tool (T108/1/2), https://www.wealdentool.com/acatalog/Online_Catalogue_Engraving_60_Degree_719.html


</ToolDefinition>
<ToolDefinition Name="15.00mm 3 flute V-Cutter 60.00 deg">
<Index>130</Index>
<Diameter>15</Diameter>
<ToolProfile>VCutter</ToolProfile>
<Flutes>3</Flutes>
<FluteLength>13</FluteLength>
<Length>72</Length>
<ShankDiameter>12.7</ShankDiameter>
<HelixAngle>0</HelixAngle>
<VeeAngle>60</VeeAngle>
<MaxRampAngle>0</MaxRampAngle>
<ToothLoad>0</ToothLoad>
<AxialDepthOfCut>0</AxialDepthOfCut>
<RadialDepthOfCut>0</RadialDepthOfCut>
<Comment>{$comment} Tool: {$tool.index} D={$tool.diameter}mm - {$tool.profile} L={$tool.length}mm Ang={$tool.veeangle}°{$endcomment}
{$comment} TOOL/CHAMFER,{$tool.diameter},{$tool.veeangle},{$tool.length}{$endcomment}
{$comment} COLOR,139,69,19 {$endcomment}</Comment>

I think the plugin assumes a perfect point.