CamBam
News:
 
*
Welcome, Guest. Please login or register.
Did you miss your activation email?
August 18, 2017, 21:00:46 pm


Login with username, password and session length


Pages: [1] 2
  Print  
Author Topic: Crop circles all over  (Read 896 times)
Anders
CNC Ewok
*
Offline Offline

Posts: 6


View Profile
« on: April 15, 2017, 18:53:16 pm »

Hello,

I am new to this forum, and also to CNC. I (try to) use CamBam as CAM programme, and Mach3 as pp.

For a couple of weeks now I have battled with crop circles, which usually originates from a wrong IJ mode setting, not unusually in the General Config in Mach3. I've had a long Machsupport (Mach3) exchange over it:

http://www.machsupport.com/forum/index.php/topic,34286.0.html

and finally downloaded CutViewer, who displays an .nc generated by CamBam v.9.8 this way (se attachment).

For some reason, CamBam 9.8 generates giantic crop circles in this job. Has anyone experienced anything like this, and what is the solution?

(I have tried out just about any aspects of the G90.1/ G91.1 // Arc Center Mode setting Absolute /Incremental in both CamBam and Mach3 (although the Gcode overrules the setting in CamBam) and as it appears in the second attachment, although the Mach3/genConfig Setting and the Gcode are in tune, still there are crop circles.)

Anders


* IMG_20170415_193056.jpg (716.14 KB, 2048x1536 - viewed 63 times.)

* IMG_20170413_172114.jpg (979.36 KB, 2048x1536 - viewed 46 times.)
Logged
lloydsp
CNC Jedi
*****
Offline Offline

Posts: 7013



View Profile
« Reply #1 on: April 15, 2017, 19:21:38 pm »

Anders, usually, also attach a copy of the offending .cb file.  Although this issue has been resolved often, having the .cb file available makes doing so easier for more difficult problems.  In this case, I think you'll get a definitive answer without it.

We have a LOT of Mach3 users here, so it should be easy for someone to state what settings they use in both CB AND in Mach-3.

Lloyd
Logged

"Pyro for Fun and Profit for More Than Fifty Years"
Anders
CNC Ewok
*
Offline Offline

Posts: 6


View Profile
« Reply #2 on: April 15, 2017, 19:33:49 pm »

At this instance, my trial version of CamBam is not able to save a cb file with any content, only the .nc...

* WOODWAVY SECTION 1B.nc (115.04 KB - downloaded 30 times.)
Logged
dh42
Administrator
CNC Jedi
*****
Offline Offline

Posts: 4562



View Profile WWW
« Reply #3 on: April 15, 2017, 19:38:56 pm »

Hello,

- When you open a file, choose the Standard G-code(*.nc) file type in CV (it will reminder this setting for the next time) .. In the Cutviewer windows you must see something like this in the top bar:

CutViewer Mill (myfilename.nc / _gcode.nci)

- In CV, crop circles can appears when the values for Maximum Arc Radius, Minimum Arc Length are not suitable for the unit that you are using. (they are set for inches by default)

try to change those values in your Mach3-cutviewer post processor and save it. (see system tab)
http://www.cambam.info/doc/dw/0.9.8/cam/PostProcessor.htm

for mm, I uses those values

Maximum Arc Radius: 10000

Minimum Arc Length: 0.01

you can also check the _gcode.nci file (it a simple text file) in the CV install folder to check if all settings are correct for IJK( CV use center start for both inc and abs arc mode), and also, why not to set the right value for the rapid move, so CV will not complain with hight feed rate. (f_rapid=xxxx)

++
David
Logged
Anders
CNC Ewok
*
Offline Offline

Posts: 6


View Profile
« Reply #4 on: April 15, 2017, 21:24:21 pm »

Thanks a lot!

This helped me greatly; I was able to generate Gcode for the CutViewer that was fine.

I'll call it a day for now, but may be back for more advice.

A good night's sleep and then...
Logged
lloydsp
CNC Jedi
*****
Offline Offline

Posts: 7013



View Profile
« Reply #5 on: April 15, 2017, 23:54:23 pm »

Anders,
I point this out to almost all new users, but I'll still do it again and again --

Please make note of how quickly you got a constructive response about your problem.

This forum excels in that respect.  I've not found any site on the internet (except one pyrotechnics site, which is my industry) where the responses are so quick and so appropriate.

I know you're running the 'trial version', but consider the support you just got before you decide to go to another CAM solution.

CAMBAM is the winner in almost all respects, and this forum is one of its strongest points.  The folks here are the BEST!

Lloyd
Logged

"Pyro for Fun and Profit for More Than Fifty Years"
Bob La Londe
CNC Jedi
*****
Offline Offline

Posts: 2843


^ 8.5 pounds on my own hand poured bait.


View Profile WWW
« Reply #6 on: April 18, 2017, 16:32:11 pm »

Absolute mode in CB and Mach3 works for 99.99998% of all applications for me.  

I currently have 4 mills and a router running Mach 3 and this works for me.  Once in a while in literally billions of lines of code I'll get an issue, but I am not completely sure its related to this.  Since I do small detailed 3D molds and lots of very short moves can be an issue you would think I'd have more problems, but I typically do not.  

I don't know why I picked absolute over incremental, but I did.  One reason I stuck with it is there seems to be only one absolute mode, and there seems to be more than one incremental mode.  

I have not done any experiments, but I do believe that I read somewhere that incremental modes take less memory and computational power.  With a computer capable of running Mach 3 reliably neither memory nor computational power should be an issue.  I have probably run a few dozens of projects now with well over a million lines of code.  I've heard Mach3's theoretical limit is about 3 million lines.  I run programs every day that are from a few to several hundred thousand lines of code.  

I'm not arguing for one over the other.  Just saying the modes (as others have said) absolutely need to match up.  No pun intended.  LOL.  

I've read several times if you set Mach 3 as your default post processor CamBam will notify Mach 3 of the IJ mode at the beginning of the code, but I prefer to make sure the mode is set to match as well.  What if I want to run part of a bit of code just to fix a part or start a program at line 517293?  Oops.  Then you skip all that setup code at the beginning.  Oops.  

As to going to another CAM.  That's kind of an empty threat.  Nobody here who helped you has any financial interest in whether or not you buy a CamBam license.  Most of us are just long time users who got some help along the way and speaking for myself feel a little obligated to help the next wave of beginners with the software.  I personally find it kind of irritating to see that threat even.  Its not meaningless to me, and makes me not to want to help.  Then I remember I was a total asshole to some of the people who helped me when I got started with CamBam, and they helped me anyway.  

I would point out that I do have an indirect reason to want people to buy a CamBam license and have new people start using it.  It makes it financially viable for Andy to keep working on it and keep adding things to it.  I am fairly proficient with CamBam and even though I have some more powerful tools available I keep coming back to it for daily paying work , because I know how to get things done with it.  It is easier to use and learn (inspite of your current frustrations) than several other CAM programs I have worked with.  It doesn't have some tools I think it desperately needs for my continued growth as a designer and machinist, but its unbelievably powerful nonetheless.  I recently spent 3 or 4 days learning how to do something in Fusion360 that CamBam couldn't quite manage, but then I came back to CamBam to do all the grunt work because it would have taken me another week to learn how to do all the rest of the stuff I already knew how to do in CamBam.  

Its a really great tool.  It doesn't do everything, but your current issues seem to be atleast partially self induced.  You don't build a house without first clearing the lot.  You can't make parts without first making sure all your settings and defaults are right.  I know it seems frustrating when you are looking at a vacant lot and all the adjoining lots have mansions on them, but if you start by clearing the trash, and then making sure the foundations is right eventually you will walk in the front door of the mansion you built carrying a box of your belongings and deciding where to put them.  
« Last Edit: April 18, 2017, 17:33:47 pm by Bob La Londe » Logged

Getting started on CNC?  In or passing through my area?
If I have the time I'll be glad to show you a little in my shop. 

Some Stuff I Make with CamBam
http://www.CNCMOLDS.com
dh42
Administrator
CNC Jedi
*****
Offline Offline

Posts: 4562



View Profile WWW
« Reply #7 on: April 18, 2017, 18:17:48 pm »

Hello

Quote
I've heard Mach3's theoretical limit is about 3 million lines.

It work with a file that is up to 10 millions lines.

Quote
I've read several times if you set Mach 3 as your default post processor CamBam will notify Mach 3 of the IJ mode at the beginning of the code

Yes, but there is a small error in the PP ; the G-code to define Distance mode and IJ mode must not be on the same line ; if it is the case, one of the code is ignored.

++
David
Logged
Bob La Londe
CNC Jedi
*****
Offline Offline

Posts: 2843


^ 8.5 pounds on my own hand poured bait.


View Profile WWW
« Reply #8 on: April 18, 2017, 18:47:00 pm »

Hello

Quote
I've heard Mach3's theoretical limit is about 3 million lines.

It work with a file that is up to 10 millions lines.

WOW!  I had definitely not heard that.  That's really cool no matter how they did it. 
Quote

Quote
I've read several times if you set Mach 3 as your default post processor CamBam will notify Mach 3 of the IJ mode at the beginning of the code

Yes, but there is a small error in the PP ; the G-code to define Distance mode and IJ mode must not be on the same line ; if it is the case, one of the code is ignored.

That is something that definitely needs to be fixed in the download versions.  It is after all supposed to be a PP for Mach3 that works with all the basic settings.  A bug like that is an issue.  For some reason it has not bit me yet that I am aware of. 
Logged

Getting started on CNC?  In or passing through my area?
If I have the time I'll be glad to show you a little in my shop. 

Some Stuff I Make with CamBam
http://www.CNCMOLDS.com
dh42
Administrator
CNC Jedi
*****
Offline Offline

Posts: 4562



View Profile WWW
« Reply #9 on: April 18, 2017, 19:08:49 pm »

Quote
WOW!  I had definitely not heard that.  That's really cool no matter how they did it.  

And tested ! ; a friend have a file with 18 millions of lines to cut (3D machining on 1x1.5 m panel).

he split the Gcode to a 10 and a 8 millions lines files and that works.
(GCode was not done with CB, we always reach the out memory error when trying)

Quote
It is after all supposed to be a PP for Mach3 that works with all the basic settings.  A bug like that is an issue.  For some reason it has not bit me yet that I am aware of.  

Because I use my own, I'm not sure that it's corrected in the last release. There is other little bugs in the PP, like the file footer that is written after the M30, so never executed and 2 small pb with the S command. It can't be set to modal, so we get unwanted Sxxx at each mop, and that slow the machining, and it is written in the Gcode at the wrong place ; the tool is still in the material when the S is executed.

++
David
« Last Edit: April 18, 2017, 19:11:26 pm by dh42 » Logged
Anders
CNC Ewok
*
Offline Offline

Posts: 6


View Profile
« Reply #10 on: April 18, 2017, 19:44:21 pm »

Thanks a lot for your attention and your interest in my small troubles.
@ Bob La londe: I don't know if some of my frustration came through in my reply to Alan, I think I expressed thankfulness, but there was absolute no threat intended. Just because I am using  the trial version, it does not mean that I am not going the purchase a license for CamBam; once things get working with no recurrent issues, I may very well do that.
Logged
lloydsp
CNC Jedi
*****
Offline Offline

Posts: 7013



View Profile
« Reply #11 on: April 18, 2017, 19:48:01 pm »

Anders,
You won't find a better solution at many times the price.  For almost every problem we've discovered in CB, there has been someone who has engineered a 'work-around'.  In the meanwhile, Andy accepts these informations, and includes the fixes for them in future revisions.

Stick with CB!  You won't be sorry.

Lloyd
Logged

"Pyro for Fun and Profit for More Than Fifty Years"
Anders
CNC Ewok
*
Offline Offline

Posts: 6


View Profile
« Reply #12 on: April 20, 2017, 11:42:23 am »

Hello,

I have a question about the holding tabs. In the documentation (and in the flyouts below the MOPs panel on the screen) it says:

"The width will be the width as measured at the thinnest part of the holding tab."

But is that width seen from 1) top as perpendicular to the cutting direction/toolpath? Or is is the width seen from 2)  top along the cutting direction/ toolpath? Or something else?

best regards

Anders
Logged
lloydsp
CNC Jedi
*****
Offline Offline

Posts: 7013



View Profile
« Reply #13 on: April 20, 2017, 12:16:06 pm »

Anders,
Width describes the distance along the middle of the toolpath. 

In other words, it's the thinnest part of the holding tab, in the horizontal plane.  One can arbitrarily make the tab as high or low in Z as one wished, also (up to the total thickness of the stock).

Lloyd

Logged

"Pyro for Fun and Profit for More Than Fifty Years"
Anders
CNC Ewok
*
Offline Offline

Posts: 6


View Profile
« Reply #14 on: April 20, 2017, 12:34:06 pm »

So the holding tab looks like a trapez seen from the side, and it's the length of the shortest of the parallel sides?
Logged
Pages: [1] 2
  Print  
 
Jump to:  

Powered by MySQL Powered by PHP Powered by SMF 1.1.19 | SMF © 2013, Simple Machines

Valid XHTML 1.0! Valid CSS! Dilber MC Theme by HarzeM
Page created in 0.155 seconds with 19 queries.

Copyright © 2008 HexRay Ltd. | Sitemap