Fixed the touch off sub routine so that the plasma cutter can now successfully run communist (metric) gcode…one less gotcha to remember…It has been tested with a part and appears to be working. Let me know if any issues arise.
Jimmy
7 Likes
Hey @Jimmy, when I would get the G-code from Fusion 360 and run it on the plasma cutter it would give an error that it cannot probe with cutter compensation turned on before every probe routine after the first one, and before the final G28 return to reference. I was having to manually edit the g-code to insert G40 before every probe routine to get the files to load. I’m not using the setup template from the Wiki, just the post processor so that might be it the cause. Either way, I opened up the post processor and added lines to insert the G40 automatically before probe routines or G28 moves. Would you like the edited post processor to put on the Wiki?
2 Likes
Nice work on the gcode editing and figuring out a solution. Would you mind trying to use everything from the wiki to see if that solves it? I believe that is the issue. The setup also sets retracts to avoid crashes from flipped up and warped parts. I cut a sheet less than a month ago and didnt have any issues. Maybe fusion 360 updated something? Feel free to post the file here in the meantime and let me know if the wiki gives you any trouble.
Thanks for the heads up,
Jimmy
1 Like
I set up my own retracts so I’ve never had problems with the warped parts, but I did figure out one other thing the template sets up is Cutter Compensation, specifically, it sets compensation type to “computer” rather than “control”. With compensation type set to “computer” it builds all the kerf offsets into the toolpath itself and doesn’t bother with any of the G40/G41 codes. With it set to “control” it sets up the offset distance and turns compensation on and off at the CNC controller level. However, I did some measuring and the CNC plasma doesn’t seem to compensate enough (or maybe at all) if you leave compensation type set to “control”. I get more precise results with it set to “computer”.
So if you use the template or set Cutter Compensation Type to “computer”, you don’t need to worry about errors or accuracy. You can turn cutter compensation off completely by setting it to “center”, which I will test later to make sure it stops the error. Instead of changing the post, I’m going to update the wiki to indicate that if you need cutter comp, set the type to “computer” and if you don’t need it then set sideways compensation to “center”. That should prevent errors in valid setups but still throw an error if someone is trying to use cutter comp in a way it won’t work.
Ref: http://help.autodesk.com/view/fusion360/ENU/?guid=GUID-C14B9F20-3A39-4930-971E-BDFE268384B9
Comps are set in the tool and are set to hypertherms default. Please dont update the wiki as we have it setup for teaching and to be as easy as possible and comp changes based on a bunch of variables. Once we get the thc working comp should be spot on.
The wiki already has the comps set to computer and the tools with the correct settings (speed, comps, tool height, pierce time, etc) Located at makeict.org/wiki/cncplasmacutter. To anyone else tuning in … Will save yourself a ton of time if you just follow the wiki
Jimmy
Link is broken, Plasma CNC page is http://makeict.org/wiki/CNCPlasmaCutter.
As for comps: the kerf width is set in the tool but whether or not cutter comp is used, which direction it compensates, and where the compensation is coded, are all set in the toolpath. THC should keep the kerf width consistent, but it won’t affect when and where cutter compensation happens.
The wiki needs to be updated to include relevant information, or at least links to the relevant information. We can add sections and organize information into “Beginner” and “Advanced” if we need to, but I don’t think it’s necessary. If you want to do the updating so it works with your teaching style, that’s fine. If you want let other community members help, but approve the changes to make sure they make sense, that’s fine too. However, MakeICT is a community for learning and sharing, not just a walk-in/walk-out tool rental. Pointing to a magic black box and rejecting further explanation doesn’t fit with MakeICT’s mission.
The relevant information that needs to go on the wiki is:
- Add “Shield 220798” to the list of consumables.
- “The rest of the parts are already on the plasma.” should be “You must provide your own electrodes and tips. There is currently a FineCut shield on the plasma cutter, but you may need to provide your own 45A/65A shield.”
- The “Fusion 360” first paragraph should include “Check the 2D Profile reference for an explanation of each of the 2D profile settings.”
- The “Templates” section should include “If you do change the tool settings and dimensions are important, using ‘Compensation Type: In computer’ under the ‘Passes’ tab is recommended for best accuracy”
- Option 1: If compensation based on G41/G42 is supposed to be working (as indicated in the PlasmaC guide), update the post-processor to my version that adds the G40 codes to allow probing to work.
OR - Option 2: Add “If ‘Compensation Type: In control’ is used anyway, your g-code will have to be manually edited to add G40 commands to turn off sideways compensation before any probe routine or G28 return to reference position” to the “Templates” section.
POST-makeict plasma v4.cps (21.9 KB)
Sorry for the brevity last night, the long story short is this has already been tested and I didn’t feel like spending an hour explaining it at 1am last night. This isn’t a black box at all (the code is available to modify) and changes that improve plasma cutter performance will be added.
Thanks for notes on the Shield 220798 and the 45/645a shield.
The rest we cover in my class and should be on the wiki (though spots are a bit hazy based on your recommendations, thanks for pointing that out, I will make some clarifications tonight). I realize classes has been sparse these last few months we have been working on improving the plasma cutter (new macros, THC, UI, etc) as class attendance was low.
There are three ways to do compensation
- By setting the “Cutter Compensation” to “in computer” and adjusting the “sideways compensation” to “left” (this is what the template “Makeict .125 lead in with kerf” does)
- By using no compensation and adjusting the “sideways comp” to center (this is what the template “makeict no lead in or kerf” does)
- Letting linuxcnc do the compensation and using “in control“ with the “sideways comp” set to “center” and g40/41 in the gcode. In theory if everything is working perfectly 1 and 3 should be the exact same with 3 providing a minor advantage in that you can finetune the compensation from linux without having to repost. However, as you found out, often they are not the same and I can give a ton more examples where this doesn’t work well, particularly with artwork loaded from Inkscape.
a. Secondly our plasma isnt accurate enough without a THC to worry about perfecting cutter comp as it can change quite a bit across the table (1/32-1/16ish). Thus, any fine tuning g40/41 would provide is lost.
From the sound of it we came to the same conclusion that in computer compensation is the way to go and if you don’t want compensation to turn it off. (Per the templates loaded to the wiki). Thus, nothing needs to be added about g40/41 as it provides no advantages at this date?
I do think we came to the same conclusion, which is even more frustrating. If a known issue had just been documented then I wouldn’t have spent my time and material figuring out why following the documentation for the software and machine didn’t give the expected results.
The known issue was documented in a way. By following the wiki and using the templates provided
this issue would have been avoided. However it was not all in vain, I updated a line in the wiki explaining the different templates and why one should be selected over the other along with a few other edits.