[ryansuperbee]

Hey guys. Does anyone have a post processor for cnc plasma? I am currently running Mach 3. I used the "Mach_3_inch" post processor that comes with Madcam. But the g-code that it produces does not turn the torch on and off in between cuts. The g-code that it generates is also overly complicated... I have a sample of g-code that works well with my cnc if that helps as well. If anyone has a post processor that works well with plasma operations, I would greatly appreciate it! Also, totally willing to pay up to $150 for anyone who can come through with a plasma post processor that will work for my machine.

[svenakela]

I think you could make a Post Processor that triggers a start/stop on Z movements. I can dig into it a bit later this week.
What do you mean with overly complicated? The path is tracking within a tolerance. Please have in mind that this is a 3D path generating tool and we normally go all around and about 3D objects, not just simple curves. With that said, the new release can make curves when there are curves to follow. I have to read up on that myself to fix my own posts so let me get back on that issue as well.

[ryansuperbee]

I think you could make a Post Processor that triggers a start/stop on Z movements. I can dig into it a bit later this week.
What do you mean with overly complicated? The path is tracking within a tolerance. Please have in mind that this is a 3D path generating tool and we normally go all around and about 3D objects, not just simple curves. With that said, the new release can make curves when there are curves to follow. I have to read up on that myself to fix my own posts so let me get back on that issue as well.

Hey! Sorry for the late reply. But thank you for responding! Right now, i have to manually edit the g-code to add the M03/M05 between each cut. Such a pain though!!! As far as the code generated, when the machine is cutting an arc, it shutters/stutters pretty bad. It should just be one smooth arc. When i look at the code generated, it seems that there more lines of code generated than necessary. Its almost as if its taking what should be one simple arc, and breaking into many small arcs and generating code for each individual arc to make one big arc. (Hope that makes sense). However, it seems to make complete circles with no problems. Thank you for helping anyway you can!

[ptoomey]

For the smooth motion issue, checkout G61 and G64 for exact stop mode and cancel exact stop. My machine did the same thing and I had to make sure I wasn't in exact stop mode so that it would look ahead a few lines and create continuous motion. The codes are different for different controllers though. On my Fagor it's G51 E.010 to make it do continuous motion with a max error of 0.010.

[svenakela]

Yes, it is important that your controller is smooth. Check these links.

https://www.cnczone.com/forums/mach-...ml#post1456594

https://www.youtube.com/watch?v=--vMC0_0Zlk

[ryansuperbee]

Hi ptoomey. Please excuse me if I sound ignorant in anyway. First, I see that when I generate g-code, on the first line I see "G64" are you saying I should delete that or change it? You simply say "checkout" and I not sure what you mean... Second, have you or has anyone figured out a way to edit the post processor in Madcam to make it automatically insert a M03/M05 between cuts?

[ptoomey]

Sorry for the vague language, it's tough because different controllers seem to use different flavors of the command. In general, G64 should set "blended path mode" or something similar in contrast to G61 which is "exact stop mode". So with G61 set, the machine would come to a stop at then end of each line, with G64 it should look ahead and try to blend the lines together into a smooth path. Some controllers use parameters after the G64 to specify maximum allowed path error or other things. For example, Tormach uses G64 P~ Q~ where P is the maximum allowed deviation from the programmed path and Q is the maximum angle between lines before it will no longer try to blend them, so sharp corners stay sharp. You would have to lookup the specific codes for your controller to see if G64 is what it wants and if so if there are some other parameters you have to set.

For the M03 and M05, the one way that comes to mind is to add them in the *TOOLPATH_CHANGE* and *FIRST_CUT* sections. I have not tried this so you would have to experiment with it to see if it works. I'm not clear on if First Cut is the first cut of each toolpath or if it's only the first cut in the file. I would assume it's per toolpath but those kinds of assumptions have bitten me in the past. I'll try to experiment with this later today if I get time and update this post.

If this works you would add the spindle stop M05 command in the *TOOLPATH_CHANGE* section of the post processor definition. This would shut off your cutter at the end of each toolpath. The only thing is that this means you have to have each cut where the cutter should turn off as its own toolpath. This may or may not be a big deal depending on the types of cuts you do and how you set them up.

Then you would put the spindle start M03 command in the *FIRST_CUT* section to start it up again before the first cut. If you need to do anything else like manually drop the z to strike the arc, dwell, or anything else specific you could add those commands here as well.

I hope this is of some help. Like I said, I'll try to experiment with this later today if possible to make sure I'm not sending you on a wild goose chase.

[svenakela]

Ryan, did you come further with this? I think I know how you can make a post processor for the plasma. I can help you with the on/off but need some input from you (like your expected program output).

Also, if this is a Rhino 6 question you can get the 2D-profiling to be super exact G-code curves instead of line approximation, it is already in version 6 but the post processors need updates.