Author Topic: GCode errors when using Mach 3 to cut an arc  (Read 408 times)

Offline Practice Makes Better

  • Ewok
  • *
  • Posts: 8
    • View Profile
GCode errors when using Mach 3 to cut an arc
« on: January 20, 2023, 01:22:44 am »
Hi, for some reason when I draw a simple arc, create a pocket then generate a GCode it will not run in my  Mach 3 Mill program, it hangs up on the second arc cutting instruction and creates this error message  "radius to the end of arc differs from the radius to start"; I have Mach selected as a post processor. Will someone point me in the right direction please?

 
« Last Edit: January 21, 2023, 01:07:55 am by Practice Makes Better »

Offline lloydsp

  • CNC Jedi
  • *****
  • Posts: 8774
    • View Profile
Re: GCode errors when using Mach 3 to cut an arc
« Reply #1 on: January 20, 2023, 02:00:02 am »
It's unusual to use an arc to form a pocket.  Circles, yes.  Ovals, yes.  Rectangles, yes.  Closed polygons, yes.  Not arcs.

Please post your .cb file.  Without it, we can't help.

Lloyd
"Pyro for Fun and Profit for More Than Fifty Years"

Offline Practice Makes Better

  • Ewok
  • *
  • Posts: 8
    • View Profile
Re: GCode errors when using Mach 3 to cut an arc
« Reply #2 on: January 21, 2023, 01:10:33 am »
Hello, I have now included my GCode, thanks.

Offline lloydsp

  • CNC Jedi
  • *****
  • Posts: 8774
    • View Profile
Re: GCode errors when using Mach 3 to cut an arc
« Reply #3 on: January 21, 2023, 01:13:58 am »
Not the g-code.  We know that's wrong, or you wouldn't have asked.  We need your CamBam file in order to help.

Lloyd
"Pyro for Fun and Profit for More Than Fifty Years"

Offline Bubba

  • CNC Jedi
  • *****
  • Posts: 3280
    • View Profile
Re: GCode errors when using Mach 3 to cut an arc
« Reply #4 on: January 21, 2023, 12:47:08 pm »
How are your settings in Mach3 and CB?
You can set either Absolute or Incremental, but both CB and Mach3 must match.

These parameters can be set in the Mach3 General config page.
Distance mode = Absolute.
IJ Mode = INC.

 
My 2¢

Win11, CB(1.0)rc 1(64 bit) Mach3, ESS, G540, 4th Axis, Endurance Laser.

Offline dh42

  • Administrator
  • CNC Jedi
  • *****
  • Posts: 7099
    • View Profile
    • Cambam V1.0 French Doc
Re: GCode errors when using Mach 3 to cut an arc
« Reply #5 on: January 21, 2023, 14:37:24 pm »
Hello

Your Gcode run fine if Mach3 if set to "Inc" for "IJmode" in Mach3 (general config)

The IJmode is not automatically set correctly by the GCode because you are not using the right post-processor and the code for setting the arc mode is not sorted (G91.1); select a Mach3 Post processor should solve the problem (and/or you can also manually set the Inc mode in Mach3, as on the picture2)

How to define a Mach3 PP as default.
http://www.cambam.info/doc/dw/1.0.0/cam/post-processor.html

Quote
I have Mach selected as a post processor. Will someone point me in the right direction please?

No, it is not the case, your Gcode has been done with the "default" PP (picture1)

++
David
« Last Edit: January 21, 2023, 14:41:41 pm by dh42 »

Offline Practice Makes Better

  • Ewok
  • *
  • Posts: 8
    • View Profile
Re: GCode errors when using Mach 3 to cut an arc
« Reply #6 on: January 22, 2023, 13:51:43 pm »
Hello DH42, I have tried several times to set my post processor to Mach 3, would you show me how to do it properly please?

Offline Practice Makes Better

  • Ewok
  • *
  • Posts: 8
    • View Profile
Re: GCode errors when using Mach 3 to cut an arc
« Reply #7 on: January 22, 2023, 14:20:13 pm »
My thanks to lloydsp, Bubba and DH42 you guys are the best. The simple solution you provided changing the General Config setting to I J Mode = INC worked. In the past I have cut arcs having one X Y origin without a problem with I J set to Absolute, the difference this time is the arc is being cut with several X Y origins; I doubt if I ever would have solved this mystery without your help. This is the best forum that I have had the pleasure of being a part of.

My best,
James

Offline Tool-n-Around

  • Storm Trooper
  • ***
  • Posts: 193
    • View Profile
Re: GCode errors when using Mach 3 to cut an arc
« Reply #8 on: January 22, 2023, 15:26:28 pm »
......How to define a Mach3 PP as default.
http://www.cambam.info/doc/dw/1.0.0/cam/post-processor.html

Ah-Hah! Think you may have answered the question I posted in a similar thread. I'll post here.

https://cambamcnc.com/forum/index.php?topic=10283.msg77317#msg77317

Best,
Kelly

Offline Bubba

  • CNC Jedi
  • *****
  • Posts: 3280
    • View Profile
Re: GCode errors when using Mach 3 to cut an arc
« Reply #9 on: January 23, 2023, 01:17:13 am »
Hello DH42, I have tried several times to set my post processor to Mach 3, would you show me how to do it properly please?

In CB, choose Tools, options then Default Postprocessor. See Attachment.
My 2¢

Win11, CB(1.0)rc 1(64 bit) Mach3, ESS, G540, 4th Axis, Endurance Laser.

Offline Practice Makes Better

  • Ewok
  • *
  • Posts: 8
    • View Profile
Re: GCode errors when using Mach 3 to cut an arc
« Reply #10 on: January 24, 2023, 01:24:21 am »
Thanks Bubba, I changed my default post processor to Mach 3 using your invaluable instructions.

Much appreciated,
James