CamBam
News:
 
*
Welcome, Guest. Please login or register.
Did you miss your activation email?
September 26, 2017, 06:24:10 am


Login with username, password and session length


Pages: [1] 2 3
  Print  
Author Topic: Break Edges Plugin  (Read 1072 times)
dave benson
CNC Jedi
*****
Offline Offline

Posts: 771


View Profile
« on: July 28, 2017, 00:21:26 am »

Hi all
Here is a small plugin designed to break the sharp edges of stock using V cutters 45/60/90 ect from your tool library.
I've tested this with 45 and 60 Deg cutters and also added some error checking so that if you forget to assign a tool or library you'll be reminded to do so.
I'll include a CB file with a tool setup to simulate in camotics tool (10) as the settings can take a little time to noodle out.
I've also included a pic of the result from camotics and the parts made from it.
The mop produced has the Tool dia and target depth set (don't change these) everything else is just like a standard mop
where you can change the other settings to suit yourself.
Dave

edit latest version with translation and traps un-selected libraries and compensates for different zoom levels.

Edit latest version larger windows to see long style, library and tool names style locked out unless you select a style library first, works with text.

* break edges test on machine with al more complicated shape.cb (13.21 KB - downloaded 9 times.)

* Break Edges 90 deg cutter tool (10).PNG (188.69 KB, 1307x576 - viewed 36 times.)

* 45 and 60 deg chamfers generated form Break Edges Plugin.png (930.58 KB, 1000x563 - viewed 43 times.)
* Break Edges.zip (14.28 KB - downloaded 8 times.)
« Last Edit: August 14, 2017, 10:53:15 am by dave benson » Logged
dave benson
CNC Jedi
*****
Offline Offline

Posts: 771


View Profile
« Reply #1 on: July 29, 2017, 13:57:10 pm »

Hi All

Today I modified and bored a couple of pockets for 6001 bearings in a NSK bearing block for my lathe and found that with using the plugin to break the edges of the pockets, that there was a slightly raised edge at the bottom of the fillet caused by the damaged tip of the 60 deg tungsten engraving cutter  I was using.
 
(I busted a few of these because the engraving mop doesn't have a spiral leadin)

So what I did was make the tool engage the work further up the cutter flutes which made these otherwise useless cutters useful, and made a nice chamfer even, with the 90 deg counter sink cutter as well.

I've replaced the old file with a new one.

Dave


* Better Chamfers with modified Break edges plugin.png (1143.91 KB, 1000x563 - viewed 28 times.)
* Break Edges.zip (12.27 KB - downloaded 12 times.)

* Better Break edges sim.PNG (42.65 KB, 1004x443 - viewed 31 times.)
« Last Edit: July 29, 2017, 13:59:25 pm by dave benson » Logged
Bubba
CNC Jedi
*****
Offline Offline

Posts: 2203



View Profile
« Reply #2 on: July 29, 2017, 16:27:17 pm »

Hi Dave, Tried your plugin,(great idea by the way) here is a what I found..

The plugin Inch Tool library is not in 'sinc' with my library. It does show mm library (default)
By looking on the screen capture, pay attention to tool #10  Wink

Thanks for trying. Cheesy


* Capture.JPG (68.44 KB, 677x489 - viewed 20 times.)
Logged
dave benson
CNC Jedi
*****
Offline Offline

Posts: 771


View Profile
« Reply #3 on: July 30, 2017, 00:16:16 am »

Hi Bubba

The tool you have selected in the the "Inch tool library" is a ball nose cutter and not a V cutter and the plugin needs a V angle to calculate the toolpaths (There's no reason that a ball nose cutter couldn't be used I just didn't think of it).
so a default cutter was chosen.

I'll add some code to catch this for now.

If you can could you post a inch CB file with a rectangle in it and I will do some further tests with real data for inch folks using the data from your library.

I can't promise anything in the next few days as I"m making up some bearing support blocks for the lathe project, but as soon as I can I'll use the software eddy put me onto to search through my snippets to find some code or plugin that has the math for Ball nose radius calculations. I think I've done this before But can't remember  Roll Eyes.

Dave
Logged
Bubba
CNC Jedi
*****
Offline Offline

Posts: 2203



View Profile
« Reply #4 on: July 30, 2017, 00:49:23 am »

Dave,

I don't think I explained this correctly. I do understand that V-angled cutter is used. The problem is with tool library selection. I use an Inch tool library, your plugin ignores that and use an mm tool library instead. So if you look carefully on picture attached in previous post snipped of my tool library is shown in the left. Take look at tool #10 selected in your plugin. Hopefully is 'clear as mud this time' Grin Grin Grin
Logged
dave benson
CNC Jedi
*****
Offline Offline

Posts: 771


View Profile
« Reply #5 on: July 30, 2017, 11:10:13 am »

HI Bubba

I've just had a look and the plugin and see what you mean so here is one that lets you select your libraries and does some more error checking.

Dave


* Break edges Inch version cb Capture.PNG (165.05 KB, 1183x585 - viewed 18 times.)

* Break edges Inch version Capture.PNG (75.66 KB, 1036x457 - viewed 24 times.)
* Break Edges.zip (12.68 KB - downloaded 13 times.)
Logged
EddyCurrent
CNC Jedi
*****
Offline Offline

Posts: 3066



View Profile
« Reply #6 on: July 30, 2017, 12:49:51 pm »

Dave,

In the context of this plugin, why do we care about Style Libary ? it seems to have no bearing on the next two selection dropdowns.
Also, the button with the small graphics, would it be useful if it toggled between, "chamfer face width" and "offset from edge" ?
« Last Edit: July 30, 2017, 12:53:17 pm by EddyCurrent » Logged
Bubba
CNC Jedi
*****
Offline Offline

Posts: 2203



View Profile
« Reply #7 on: July 30, 2017, 13:49:43 pm »

If you can could you post a inch CB file with a rectangle in it and I will do some further tests with real data for inch folks using the data from your library.
************************************

Sure, 

* Break Edges_INCH.cb (4 KB - downloaded 8 times.)
Logged
dave benson
CNC Jedi
*****
Offline Offline

Posts: 771


View Profile
« Reply #8 on: July 30, 2017, 14:29:36 pm »

Hi Eddy

In the context of this plugin, why do we care about Style Library ? it seems to have no bearing on the next two selection drop downs.

Eventually I wanted to be able to select a style  library and then a style, so that the mop would be fully specified this way (I have style 3mm in al) that if I select, then everything is specified including feed rates leadin ect.
But I have friends that use CB and  don't use style libraries at all, so I wrote the plugin with them in mind.

Also, the button with the small graphics, would it be useful if it toggled between, "chamfer face width" and "offset from edge" ?

Yes that was the thinking, that's why it is a button and not a label, but there's a few issues to think about :

David pointed out a fillet is specified as a (1mm by 1mm or a 2 mm x 2mm) from the top and side edges and with a 90 deg  cutter (effectively 45 deg chamfer on the edge your cutting)  you can do this with one textbox but with a 60 or 30 deg V-cutter  or a ball nose cutter you may need some extra textboxes for some extra data to specify where you want to position radius of the scallop of the ball nose tool to make edges like woodworkers might do with a spindle router form tool without resorting to 3D.

Right now I'm in the middle of the lathe X axis fit up and am keen to press on with it, which will probably take 3 or 4 days, then I'll have to save up for a control box to put the controller and inverter in so I'll have some free time to add some things to plugin.

It's good  to have people with some insight make suggestions, be it from a programming or machining point of view.
thanks Bubba That'll help alot.

Dave
Logged
kvom
CNC Jedi
*****
Offline Offline

Posts: 1383


View Profile
« Reply #9 on: July 30, 2017, 15:51:15 pm »

I'll make a few comments here for what it's worth.

What you're doing is mainly a very basic chamfer plugin.  What might be most useful is an actual chamfer plugin that would require more elaboration, and would need to be able to specify more about the tool geometry and the cut itself.  I'm not sure if your ambition was to do much more than what you've done already.

For tool geometry, in addition to the taper angle, you'd want to handle bits that have a flat tip as well as a complete point.  Also, the engagement distance from the tip to allow cutting with the thicker part of the tool.

For the actual cut, multiple passes may be needed, as are specifiable with cut width and step over.  Plus you'd want to be able to show the cutwidth display as inside the profile.  I also tend to use lead ins for chamfers.

All these things are what I calculate manually before coding a profile MOP.

Logged
EddyCurrent
CNC Jedi
*****
Offline Offline

Posts: 3066



View Profile
« Reply #10 on: July 30, 2017, 16:13:59 pm »


It's good  to have people with some insight make suggestions, be it from a programming or machining point of view.

Dave

Dave, it's good to have comments of any kind  Wink
Logged
dave benson
CNC Jedi
*****
Offline Offline

Posts: 771


View Profile
« Reply #11 on: July 31, 2017, 01:11:07 am »

Hi Eddy and Kvom

Quote
Dave, it's good to have comments of any kind  

Ha Ha I recall a quote from a fading Hollywood movie star (can't remember who it was now  ) that went something like, The only thing worse than being “talked about “ was “not being talked about”.

Unlike a few of the other plugins that I've written, which I did for a bit of fun and to learn something new, this plugin was borne of a genuine need.

 As in descending order I work with Steel/Aluminium/Eng plastics and have to break the edges
as a matter of routine, sometimes for aesthetics but mostly for safety.

Quote
I'm not sure if your ambition was to do much more than what you've done already.

It wasn't really, as I cut out parts of various sizes from  1.5 mm to 16 mm thick al on a per job basis, a one size fits all  chamfer wasn't appropriate and calculating the chamfers for each individual part on the sheet gets old quickly.

The latest version does cut a bit further up the tool as a bit of testing on the machine showed that
the very bottom of the tool tip left another edge to break,  and also the surface speed at the tip of the tool is very low and  the finish wasn't very good, and as I don't have a high speed spindle I couldn't do much about this.

To address this I have added a small offset (negative roughing clearance) and added a bit to the tool depth of the tool path, but there are some constraints here depending on the geometry of the tool.

For example my 90 Deg countersink is a large tool both in depth and width, and so I can cut further up the flank of the tool (I did this in the last version) and  there was a remarkable improvement in finish, however with the 60 and 30 deg cutters you are somewhat constrained by the geometry of the tool itself.

As to multiple passes, the plugin produces a standard profile mop with the Tool Dia, Roughing Clearance and Depth of Cut fields calculated and filled in, and so anything else (like leadin's for example)  can be set as you need.  I always use the spiral leadin as a matter of course.

I could set the spiral leadin when the mop is generated, but because our machines and materials are different there might not be a one size fits all "Depth Increment" that I could use for the spiral leadin's.
 
But I'm not a machinist by trade and am happy to take advice on this.

Dave
« Last Edit: July 31, 2017, 01:13:43 am by dave benson » Logged
Bubba
CNC Jedi
*****
Offline Offline

Posts: 2203



View Profile
« Reply #12 on: July 31, 2017, 02:20:49 am »

Dave,

From my experience by doing this for living,(happily retired now)the  depth increment is unnecessary. I have always cut chamfer's in one pass, sometimes climb milling. Always with good result.
Logged
dave benson
CNC Jedi
*****
Offline Offline

Posts: 771


View Profile
« Reply #13 on: August 08, 2017, 11:18:48 am »

HI All

OK here's a new version of the plugin where you can use a pre-configured style to make your break edges mop from, (this gives you the ability to totally specify all of the parameters ) so that you don't have to create a mop and then enter the feeds and speeds leadin's ect.

First you have to create a new style or styles in your style library like the picture below.

If you want to use styles then:
Then load up the plugin.
Select the geometry to apply the mop to.
Select a style library.
Select a style.
Select a tool Library.
Select a tool.
 
Click create mop.
One thing to remember is that if you select a circle or arc (which are not polylines), then the mop will not include them, you must then right click on the mop and select add drawing objects to include them in your mop.

I could have had the plugin convert these circles and arcs to polylines and include them in the mop
But if you had  previously used them in other mops you would have to re-enter them into those mops, so I left this choice for you to do yourself.

If  there's no issues found in the next couple of days then I'll call it done, and as promised will start on the                
 ” IsThinking” issue with Eddy.

Dave


* Break Edges with styles showing style library.PNG (124.82 KB, 892x610 - viewed 16 times.)

* Break Edges with styles.PNG (115.67 KB, 908x517 - viewed 16 times.)
* Break Edges.zip (13.61 KB - downloaded 12 times.)
« Last Edit: August 08, 2017, 11:33:24 am by dave benson » Logged
EddyCurrent
CNC Jedi
*****
Offline Offline

Posts: 3066



View Profile
« Reply #14 on: August 08, 2017, 11:46:17 am »

Dave,

I found the thinking setup is an EditMode.
Logged
Pages: [1] 2 3
  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 0.171 seconds with 18 queries.

Copyright © 2008 HexRay Ltd. | Sitemap