G93 for Rotary LinuxCNC Post Processor

This forum is for requests and queries about machine tool support for Vectric Products

G93 for Rotary LinuxCNC Post Processor

Postby rjshust » Mon Sep 16, 2019 10:53 pm

I have a traditional CNC, and now I have recently started working with rotary CNC woodworking. My machine has X, Z, and A axis. I am currently using vcarve pro 9.5. Both my machines run on LinuxCNC.

My issue – when using rotary gcode straight out of vcarve, the rotary speeds are all over the place. Often VERY slow, but then sometimes it will suddenly go crazy fast.

I understand that as of version 9.5 vectric products now can work with G93. I currently run my gcode through a free product called “Rapid Rotary” (there is a nice youtube video showing the issue, and showing the software). This software does a good job converting the code to work with the G93 command, and if I cannot get the PP to work, I will still be ok. I would much prefer elimination that step, and having more control using the vectric PP.

I have tweaked my PP for basic changes, but I do not understand how to change the PP to work with the G93 command.

Is there already a PP out there I can tweak to work with LinuxCNC, or can someone explain how to convert my existing PP to work with G93.
rjshust
 
Posts: 4
Joined: Wed Jul 19, 2017 5:14 pm
Model of CNC Machine: Sidewinder

Re: G93 for Rotary LinuxCNC Post Processor

Postby gregk » Tue Sep 17, 2019 12:46 pm

If you have a working rotary PP for your machine, enabling G93 inverse time mode should be relatively straight-forward. To enable it you need to make following modifications:
  • Add following code to enable inverse time mode in the output
    Code: Select all
    INVERSE_TIME_MODE = YES
  • Enable inverse time mode on your controller (e.g. by adding G93 command in HEADER
  • Add inverse time variable:
    Code: Select all
    VAR INVERSE_TIME = [FI|A| F|1.1]
  • Add inverse time output for relevant moves, e.g.: by using [FI] instead of [F] in G1 moves
    Code: Select all
    +---------------------------------------------------
    +  Commands output for feed rate moves
    +---------------------------------------------------

    begin FEED_MOVE

    "G1 [X] [Y] [Z] [FI]"

I hope that helps. In any case if you decide to modify the post processor make sure that you've make a copy of the original file and be sure to inspect and verify generated g-code to ensure that it works the way you would expect, before sending it to the machine. Performing an air cut my also be a good idea.

Greg K
gregk
Vectric Staff
 
Posts: 73
Joined: Mon Mar 05, 2018 12:34 pm
Model of CNC Machine: None

Re: G93 for Rotary LinuxCNC Post Processor

Postby rjshust » Tue Sep 17, 2019 5:50 pm

Thank you so much.

I will plug this in tonight and take a look at the gcode generated. If it looks good, I will try it on the machine this weekend.

Thanks again,
Rob
rjshust
 
Posts: 4
Joined: Wed Jul 19, 2017 5:14 pm
Model of CNC Machine: Sidewinder

Re: G93 for Rotary LinuxCNC Post Processor

Postby rjshust » Wed Sep 18, 2019 3:13 am

I am getting error:

F1
Unknown variable name
On line 144 of file
C:\-----------------------------------
"G01 [X] [Y] [Z] [F1]"



Any ideas?
Attachments
LinuxCNC_Wrap_Y2A_inch test.pp
Post P
(5.48 KiB) Downloaded 15 times
rjshust
 
Posts: 4
Joined: Wed Jul 19, 2017 5:14 pm
Model of CNC Machine: Sidewinder

Re: G93 for Rotary LinuxCNC Post Processor

Postby gregk » Wed Sep 18, 2019 8:34 am

Looks like you placed [F1]] instead of [FI]. The second character is 'I' as in 'ice'. I can see that in this font both characters look almost the same.

There a few more things that needs changing:
  • In header section the postp was still issuing G94. I changed it to G93.
  • I added G94 in the footer, to restore the more usual feed rate mode after toolpath is finished.
  • The [F] have to be replaced with [FI] for every move, not only the FEED_MOVE. I added changed it for FIRST_FEED_MOVE as well.


Please find the PP with all of the above corrections:
LinuxCNC_Wrap_Y2A_inch test.pp
(5.52 KiB) Downloaded 23 times


Greg K
gregk
Vectric Staff
 
Posts: 73
Joined: Mon Mar 05, 2018 12:34 pm
Model of CNC Machine: None

Re: G93 for Rotary LinuxCNC Post Processor

Postby rjshust » Wed Sep 18, 2019 6:54 pm

Thank you.

The gcode looks good. I cannot test on the machine till the weekend, but from what I can see, it looks very similar to what that other program was generating.
rjshust
 
Posts: 4
Joined: Wed Jul 19, 2017 5:14 pm
Model of CNC Machine: Sidewinder


Return to Post Processors

Who is online

Users browsing this forum: No registered users and 2 guests