Hello Guest it is March 28, 2024, 12:59:18 PM

Author Topic: Toolchange not supported by post processor  (Read 5258 times)

0 Members and 1 Guest are viewing this topic.

Toolchange not supported by post processor
« on: August 15, 2014, 10:30:25 AM »
Hello,

I am using Artcam pro to generated G-code with arcs, whenever I try and generate the code with more than one tool I get a warning to say that my post processor does not support toolchanges. Is there something I can add to the post processor file to sort this? It is not a huge issue but it does mean I am not using the machine and it's facilities to it's full potential. It would also save me having to generate several files for one job.

Many thanks,

Stu

Offline ger21

*
  • *
  •  6,295 6,295
    • View Profile
    • The CNC Woodworker
Re: Toolchange not supported by post processor
« Reply #1 on: August 15, 2014, 11:31:14 AM »
Check the ArtCAM manual forhow to edit post processors, but you need to add something like this to your post processor:

TOOLCHANGE = "M6 [T]"
TOOLCHANGE = "M3"
Gerry

2010 Screenset
http://www.thecncwoodworker.com/2010.html

JointCAM Dovetail and Box Joint software
http://www.g-forcecnc.com/jointcam.html
Re: Toolchange not supported by post processor
« Reply #2 on: August 15, 2014, 01:47:42 PM »
Thanks for that. The manual isn't great but having had a look at some of the other post processors it would make sense to put that at the end of the file. I would imagine that it goes through each process and determines if there is a new tool after each operation.

Offline ger21

*
  • *
  •  6,295 6,295
    • View Profile
    • The CNC Woodworker
Re: Toolchange not supported by post processor
« Reply #3 on: August 15, 2014, 02:08:59 PM »
There also should be an S in brackets in there with the M3, but the forum wouldn't take it in the correct format.
Gerry

2010 Screenset
http://www.thecncwoodworker.com/2010.html

JointCAM Dovetail and Box Joint software
http://www.g-forcecnc.com/jointcam.html
Re: Toolchange not supported by post processor
« Reply #4 on: August 15, 2014, 03:46:29 PM »
START = "T[T] M6"
START = "[ S] M3"

TOOLCHANGE = "T[T] M6"
TOOLCHANGE = "[ S]  M3"
« Last Edit: August 15, 2014, 03:55:51 PM by Ya-Nvr-No »
Re: Toolchange not supported by post processor
« Reply #5 on: August 15, 2014, 05:09:28 PM »
Thanks again, that seems to have done the trick. Do I need to add an M05 before the M6 or does the M6 have a macro that will stop the spindle when it comes for a toolchange?

Offline ger21

*
  • *
  •  6,295 6,295
    • View Profile
    • The CNC Woodworker
Re: Toolchange not supported by post processor
« Reply #6 on: August 15, 2014, 05:56:19 PM »
You should add another toolchange line with the M5 before the M6.
Gerry

2010 Screenset
http://www.thecncwoodworker.com/2010.html

JointCAM Dovetail and Box Joint software
http://www.g-forcecnc.com/jointcam.html
Re: Toolchange not supported by post processor
« Reply #7 on: August 15, 2014, 06:32:22 PM »
I haven't had a M5 before my tool changes in ArtCam in years though I do have one at the END

added one of my posts below
I added the .txt as not sure it would post here

Offline ger21

*
  • *
  •  6,295 6,295
    • View Profile
    • The CNC Woodworker
Re: Toolchange not supported by post processor
« Reply #8 on: August 15, 2014, 06:35:31 PM »
If you have Mach3 set to "Stop Spindle, Wait for Cycle Start", then you don't really need the M5. But it's probably good practice to have it in there.
Gerry

2010 Screenset
http://www.thecncwoodworker.com/2010.html

JointCAM Dovetail and Box Joint software
http://www.g-forcecnc.com/jointcam.html
Re: Toolchange not supported by post processor
« Reply #9 on: August 18, 2014, 04:33:25 PM »
Thanks for your help. I think I have something suitable I will give it a go tomorrow.