How to create Centroid Plasma G code with Sheetcam

[Joey]

I've Made a walk-thru video on Importing the Centroid Plasma Post into SheetCam. I also walk through Importing A Simple DXF into SheetCam and turning it into G-Code for Acorn Plasma.


Video link is https://photos.app.goo.gl/Ggzum3SUvy7XasHKA

[ShawnM]

Thanks Joey, it was interesting to see how sheet cam works. I have downloaded the demo version and wanted to try to start to learn it but not sure I have the time to learn yet another program. I like that it is plasma specific and some of its features but again learning more programs takes time.

I'll be converting my Shop Sabre Sidekick 10 plasma table with a Hypertherm 85 shortly to Acorn as a beta tester. I've been using Vectric software for years now and was able to take to take the WinCNC PP for plasma and the Shop Sabre Plasma PP and sort of combine the two for a plasma PP that works in the Vectric software for my machine. I have both Cut 2D and Vcarve and my PP works really well. I can import my DWG file into Vectric and create the cut paths (layers like Sheetcam) and generate g code using the custom PP I created. I did a similar setup in the Vectric software by creating a tool library that basically is a list of tools that simply define the kerf width only. All the other setting like in Sheetcam are irrelevant because the current WinCNC controller takes care of all the other settings like the way Centroid is doing it with the "Profile Manager". I love this setup and how the software takes care of everything. No need to create other G code simply because I changed material.

Thanks again for the video and I'm excited to get started with the Acorn Plasma very soon.

[Joey]

Thanks for the feedback!

[jcoldon]

the only problem. Is Acorn plasma took the setting power of sheet cam . Away . they only using it for x y axis . all the other speeds are in the screen
and only 1 x y speed in acorn plasma. so there no way to layer mutli speeds or do other settings that are in sheet cam. i been using sheet cam for 10 years
it does a lot more then just set start points lead in . dun right you can realy fine tune cuts with the propper settings and turn on codes in controller
Air plasma one setting does not fit all . you guys see that once you start cutting

[ShawnM]

Here is a link to download the latest Centroid SheetCam Plasma Post Processor that we are testing with

https://www.centroidcnc.com/centroid_di ... oller.html

Hey Joey, it says "failed, no file" when I try to download it. Just FYI. I don't use sheetcam but was curious to see their PP. Keith send me one but it actually looks like the code to write the PP but I've never seen a sheetcam PP before so maybe it's that complicated. I don't plan on using sheetcam either. No time to learn yet another program. Vectric programs work just fine for plasma.

I'll be at the shop tomorrow and can share my PP that I use for Vectric software. It'll work with Cut2D and Vcarve Pro.

[cnckeith]

I'll be at the shop tomorrow and can share my PP that I use for Vectric software. It'll work with Cut2D and Vcarve Pro.

great, i'll add it to the downloads page for others to use!

[ShawnM]

Got, that's the same thing Keith sent me.

The Vectric one is a little easier to read and edit but I say that because I'm used to editing Vectric PP's. I'll clean it up and comment it as much as possible so others can use and edit it if necessary.

[cnckeith]

the only problem. Is Acorn plasma took the setting power of sheet cam . Away . they only using it for x y axis . all the other speeds are in the screen
and only 1 x y speed in acorn plasma. so there no way to layer mutli speeds or do other settings that are in sheet cam. i been using sheet cam for 10 years
it does a lot more then just set start points lead in . dun right you can realy fine tune cuts with the propper settings and turn on codes in controller
Air plasma one setting does not fit all . you guys see that once you start cutting

Jeff,

did some testing of slow down in arcs etc......we inherently support other feedrates other than the profile feedrate in the part program G code.

To slow down an arc or group of arcs, all you have to do is insert the feed rate you want that is different from the profile feedrate.

For example. Say the Profile feedrate is 200 ipm.....but we want 100 ipm in the circles...

;Filename: Centroid_test_hook.tap
;Post processor: Centroid Plasma THC (1) (1).scpost
;Date: 01/10/2021
G20 ;Units: Inches
G90
M65
;Part: Metric Hook
;Operation: Inside Offset, Inside Circles, T2: Plasma, 1.501 mm kerf
G0 X2.5312 Y0.7983
M61 ; < M61 picks up the feedrate data from the profile that is currently loaded>
G3 X2.6516 Y0.7178 I0.1004 J0.02 F100 ;<Feedrate for small arc came from Sheetcam, Profile feedrate was 200 but is now changed to 100 for this arc and the arcs below it>
G3 I-0.0696 J0.0696
G3 X2.5711 Y0.8382 I-0.1004 J0.02
M62
G0 X4.1172 Y0.7983
M61 < M61 picks up the feedrate data from the profile that is currently loaded, feedrate is now changed from F100 back to the Profile feed rate (200 ipm for this example)>
G3 X4.2376 Y0.7178 I0.1004 J0.02
G3 I-0.0696 J0.0696
G3 X4.1571 Y0.8382 I-0.1004 J0.02
;Operation: Outside Offset, Outside Edge, T2: Plasma, 1.501 mm kerf
M62

This works as is right now....You can do it as a test.... just hand edit the g code and put the F commands where you want them....

____________________


Now to automate it using the post processor to reset the profile feedrate after selected geometry slow down....This is how we would go about it..
see the g code example below with different feedrates on just sections of the whole path. effectively slowing down only in the cad/cam selected sections of the part path. but then returning to the profile feedrate for the sections that we don't want to slow down.

G0 X1.8424 Y0.1258
M61 ;< M61 picks up the feedrate data from the profile that is currently loaded>
G3 X1.8515 Y0.3066 I-0.0859 J0.0949 F100 ; < F command inserted by Sheetcam to slow down this arc to 100 ipm>
G2 X1.7421 Y0.5906 I0.3139 J0.2839
G1 Y0.748 F<FEEDRATE> ; <F command inserted by Sheetcam returns Feedrate to Profile specified feedrate so all g code below, where F<FEEDRATE> is the current loaded Profile feedrate >
G3 X1.378 Y1.1122 I-0.3642 J0 F100
G1 X0.7874 F<FEEDRATE>
G3 X0.4626 Y0.7874 I0 J-0.3248
G1 Y0.5906
G2 X0.1673 I-0.1477 J0
G1 Y0.7874
G2 X0.7874 Y1.4075 I0.6201 J0 F100
G1 X3.9679 F<FEEDRATE>
G2 Y0.1673 I0 J-0.6201 F100
G1 X2.1527 F<FEEDRATE>
G2 X2.1505 Y0.1674 I0 J0.0295
G1 X2.1238 Y0.1694
G1 X2.123
G2 X1.8515 Y0.3066 I0.0423 J0.4211
G3 X1.6707 Y0.3157 I-0.0949 J-0.0859 F100
M62

the post processor will have to be edited to support slower feedrate insertion for selected geometry and return the feedrate to the profile settings using the F<FEEDRATE> command. so that will be the next iteration.

Best regards,

Keith

[jcoldon]

OK thanks keeth once the mod dun for the post processor .
Were will the feed rate be inserted in sheet cam second layer profile . or codes. or in the post processor
i use code in sheet cam any circle below 1 inch THC off speed slow 60 percent and setup corectly it incert the codes like the uccnc code i sent you.

[cnckeith]

OK thanks keeth once the mod dun for the post processor .
Were will the feed rate be inserted in sheet cam second layer profile . or codes. or in the post processor
i use code in sheet cam any circle below 1 inch THC off speed slow 60 percent and setup corectly it incert the codes like the uccnc code i sent you.

hello.
not necessary to use sheetcam to force torch off. Centroid software does this automatically.

Use the Anti Dive Velocity control in the THC config menu.

from the Centroid Plasma Manual.

Velocity Anti Dive Ratio is Velocity based Anti Dive control.
Velocity based anti-dive will prevent THC motion (THC OFF) when the actual
X-Y velocity of the machine is less than the specified %. Used to turn off THC
automatically when entering tight arcs or turn arounds.

this control will automatically turn off the THC in small arcs when the machine feedrate drops below the percentage you set.