Rounded Toolpath issue

This forum is for general discussion about Aspire
Post Reply
JCman
Posts: 6
Joined: Mon Aug 31, 2020 1:53 pm
Model of CNC Machine: Bobs Evolution 3

Rounded Toolpath issue

Post by JCman »

If been using this gadget for some time now and it has worked perfectly until the new version 11 came out. Here is my problem. Ill generate the toolpath by selecting the radial option, ill load my square stock on to my machine and using UGS ill run the file. Before the update, the bit would lift and the rotary axis would rotate then the bit would lower and start rounding my stock. Now the bit doesn't lift , the rotary axis rotates and the bit buries its self into the first corner because it failed to lift. I tested this on my other computer with version 10.5 and it works perfectly. Hope this makes since. If someone with a rotary axis could test this and see if it happens to you, i would appreciate it. I have tried setting my rapid Z gap above my material higher but doesn't help.

Thanks!

User avatar
Rcnewcomb
Vectric Archimage
Posts: 5864
Joined: Fri Nov 04, 2005 5:54 am
Model of CNC Machine: 24x36 GCnC/WinCNC with ATC
Location: San Jose, California, USA
Contact:

Re: Rounded Toolpath issue

Post by Rcnewcomb »

Have you compared the output files between the versions?

Here is what I get after the spindle On command. Mine uses a G53 to send my Z to the top before it starts cutting.

Code: Select all

 [TOOLPATH NAME: Rounding Toolpath]
 F120 XY [SET FEEDRATE FOR X AND Y]
 F120 Z [SET FEEDRATE FOR Z]
 F{(114.5916)*(120)/(3.000)} A [SET FEEDRATE FOR A]
  
 G53 Z0 [LIFT Z TO TOP]
 G0 X0 Y0
 
 G0 A-49.727110 Y0.000000
 G0 Z3.537
 G1 A-49.727110 Y0.000000 Z2.621320
 G1 A-49.727110 Y28.000000 Z2.621320
- Randall Newcomb
10 fingers in, 10 fingers out, another good day in the shop

JCman
Posts: 6
Joined: Mon Aug 31, 2020 1:53 pm
Model of CNC Machine: Bobs Evolution 3

Re: Rounded Toolpath issue

Post by JCman »

Thanks for the reply.
Im not good at reading G-Code, but this is what i have for line 53 G1X254.0000F1270.0.
However, here is what i have on line 4 G0X0.0000A0.0000 in the new version 11.
Here is what i have in version 10.5 on line 4 G0Z15.7013.

Like i said, im not good at reading G-Code, but it looks like in version 10.5 line 4 starts with G0Z and in version 11 line 4 starts with G1X.

I really believe its a issue in version 11 when generating G-Code for the rounded toolpath. Maybe some one from Vectric can look into this.

User avatar
martin54
Vectric Archimage
Posts: 7332
Joined: Fri Nov 09, 2012 2:12 pm
Model of CNC Machine: Gerber 48, Triac PC, Isel fixed gantry
Location: Kirkcaldy, Scotland

Re: Rounded Toolpath issue

Post by martin54 »

It may be a change in the post processor that V11 is using the post processor that I am using for UCCNC has a different behavior & I am not sure how to change it, hasn't caused me any problems but it moves the z down before moving x & y to the start position so possibly a post processor issue rather than a V11 problem.
Other thing you might want to look at is the z home position rather than the rapid z hight as that may have changed with the new version :lol: :lol: :lol:

User avatar
Rcnewcomb
Vectric Archimage
Posts: 5864
Joined: Fri Nov 04, 2005 5:54 am
Model of CNC Machine: 24x36 GCnC/WinCNC with ATC
Location: San Jose, California, USA
Contact:

Re: Rounded Toolpath issue

Post by Rcnewcomb »

Maybe some one from Vectric can look into this.
The best way to ensure to get an official Vectric response is to send an email to support@vectric.com
This is a user-to-user support forum, but sometimes the Vectric staff does see and respond.
Im not good at reading G-Code
If you can put both output files into a ZIP file and upload them here then we can take a took.
- Randall Newcomb
10 fingers in, 10 fingers out, another good day in the shop

JCman
Posts: 6
Joined: Mon Aug 31, 2020 1:53 pm
Model of CNC Machine: Bobs Evolution 3

Re: Rounded Toolpath issue

Post by JCman »

Ok, i have attached the two files labeled version 10.5 and 11.

Thank you for helping me out on this.
Attachments
Rounding Toolpath Version 10.5.zip
(893 Bytes) Downloaded 49 times
Rounding Toolpath Version 11.zip
(923 Bytes) Downloaded 44 times

User avatar
Rcnewcomb
Vectric Archimage
Posts: 5864
Joined: Fri Nov 04, 2005 5:54 am
Model of CNC Machine: 24x36 GCnC/WinCNC with ATC
Location: San Jose, California, USA
Contact:

Re: Rounded Toolpath issue

Post by Rcnewcomb »

There is a difference in order of operations between the post processor you use for the 10.5 code vs the V11 code.

The quick fix is to copy the 10.5 post processor to your V11 installation.

Lines 4 and 5 are in different order.
In 10.5 it first does a rapid move of the Z (line 4) and then does a rapid move of X and A (line 5). The V11 post processor swapped those operations.
Attachments
Screen Shot 2021-08-04 at 7.15.07 AM.png
- Randall Newcomb
10 fingers in, 10 fingers out, another good day in the shop

User avatar
dealguy11
Vectric Wizard
Posts: 2459
Joined: Tue Sep 22, 2009 9:52 pm
Model of CNC Machine: Anderson Selexx 510
Location: Henryville, PA

Re: Rounded Toolpath issue

Post by dealguy11 »

Based on Randall's analysis, this looks like another instance where migrating to a new post-processor in the new release has resulted in unexpected changes. There have been a bunch of posts with this theme over the last couple of releases.

In most cases, if a post-processor is working correctly with your machine in an older version of Vectric software there is no reason to use a newer version of the post-processor. The older one should continue to work fine and it saves a lot of headaches trying to figure out what changed. If you use a customized post-processor, like I do, then it's pretty critical that you don't change post-processors.

The easiest way to make sure your post-processor doesn't get blown away by an upgrade is to click "Open Application Data folder" under the file menu, navigate to the earlier version of the Vectric software, copy the post-processor that works, navigate back to the current version and paste the post-processor in the "My_PostP". You will then need to associate it with your machine.

Unless your post-processor is already throwing off errors, or you've upgraded your machine controller, then I can't think of many good reasons to update just because different post-processors came out in the new version.
Steve Godding
Not all who wander (or wonder) are lost

CRV
Vectric Alumni
Posts: 16
Joined: Wed Mar 04, 2020 10:04 pm
Model of CNC Machine: N/A

Re: Rounded Toolpath issue

Post by CRV »

Hello JCman

Can I ask that you get in touch with support about this issue? We would like to take a look at this more in depth please.

If you can email support@vectric.com and send us a copy of the 10.5 post that works well for you so that we can take a look at it and go from there. Also if you can send us a .CRV file in with the issue and let us know the gadget version you are using there and if possible send us a copy of the gadget that would be great.

Thanks

Chris

JCman
Posts: 6
Joined: Mon Aug 31, 2020 1:53 pm
Model of CNC Machine: Bobs Evolution 3

Re: Rounded Toolpath issue

Post by JCman »

Thanks Chris, i sent the email.

Post Reply