QCAD.org Forum

Before I pony up for the whole package, can someone chime in on the Cam side of things? I specifically want to run this with the Langmuir Crossfire Pro plasma table. The offer the post processor for sheetcam, but I was wondering if I could save a step by using the Qcad/cam to do both part design and G-code generation.

There is no post processor out of the box for this controller (FireControl). However, it looks like standard G-Code, probably with some extra codes. If you can provide an example file that works on your machine, we can tell you more.

Thanks, I won't get my machine until June. I will update this thread at that time.

Here's the same part with fusion post and QCAD. The difference is fairly simple... I have an automatic height module so there is a block of code before each cut which basically is torch-height adjustment and the pierce process.


If you can get post set up, I'll post about this on the Langmuir forums and make sure people know they can use QCAD seamlessly with the CrossFire Pro. I think there's an upside for your efforts.

Is there any documentation/guidance/examples for writing postprocessing code? If you can't provide a postprocessor, perhaps I could build it for you.



Here's a simple part with fusion360 + Langmuir post

[quote](v1.6-af)
(top and bottom, 2pc)
(Machine)
( vendor: Langmuire Systems)
( model: Pro)
( description: CrossFire Pro)
G90 G94
G17
G20
H0

(2D Profile6)
G0 X-1.5108 Y-0.0625
G92 Z0.
G38.2 Z-5. F100.
G38.4 Z0.5 F20.
G92 Z0.
G0 Z0.04 (IHS Springback + Backlash)
G92 Z0.
G0 Z0.15 (Pierce Height)
M3
G4 P0.6
G0 Z0.063 (Cut Height)
H1
G1 X-1.4025 Y0. F20.
G3 X-1.5975 I-0.0975 J0. F20.
G3 X-1.4025 I0.0975 J0.
G1 X-1.5108 Y0.0625
H0
M5
G0 Z1.

G0 X-1.3941 Y-0.4036
G92 Z0.
G38.2 Z-5. F100.
G38.4 Z0.5 F20.
G92 Z0.
G0 Z0.04 (IHS Springback + Backlash)
G92 Z0.
G0 Z0.15 (Pierce Height)
M3
G4 P0.6
G0 Z0.063 (Cut Height)
H1
G1 X-1.4415 Y-0.288 F20.
G1 X-1.5373 Y-0.275
G2 Y0.275 I0.0373 J0.275
G1 X1.2463 Y0.6523
G1 X1.25 Y0.6525
G1 X1.75
G2 X1.7775 Y0.625 I0. J-0.0275
G1 Y-0.625
G2 X1.75 Y-0.6525 I-0.0275 J0.
G1 X1.25
G1 X1.2463 Y-0.6523
G1 X-1.4415 Y-0.288
G1 X-1.518 Y-0.3868
H0
M5
G0 Z1.

M30
(PS20)[/quote]



Here's what I got from QCAD



[quote]G0 Z1
G0 X0.0884 Y-0.0884
T1 M6
S100 M03
G0 Z2
G1 Z-4 F20
G3 X-0.0884 Y0.0884 I-0.0884 J0.0884
G3 X0.0884 Y-0.0884 I0.0884 J-0.0884
G1 Z2
G0 X3 Y0
G1 Z-4
G1 Y-0.625
G1 X2.75
G1 X-0.0336 Y-0.2477
G2 Y0.2477 I0.0336 J0.2477
G1 X2.75 Y0.625
G1 X3
G1 Y0
G1 Z2
G0 Z1
M30[/quote]

Hi,
Seems that 'Pluge' = and 'Retract' = Should be easy, any main header too.
For the plunge section the 'Post' itself needs a few extra parameter fields.
Not that big of a deal.

Apart from that I can't make out on the fly if the travelled paths are equal.

Regards,
CVH

So I've hacked together a postprocessor in perl. It does static, wiggle, ramp, and spiral pierce. Hops over slag, if you want, etc. It detects the beginning and end of profiles and puts in pierce, retract, and feed settings. Wrote a bunch of test patterns for the Razorweld Cut45 by hand and post-processed with no problem.

Now, I'm trying to use CAM output from QCAD for a non-test piece. There's a stupid G41 in the output. Stupid because it doesn't make sense and a real problem because the FireControl doesn't know what to do with G41. I moved the part so the corner of the part is on the origin---still have a G41 command. I move the start point of the polyline to the origin. Now the G41 offset is 0.00

Does anyone know how to suppress this G41 output? I want to generate several tool paths but they can't all start on the origin. Also, on a simple part, I didn't find G41 in the output.

Also, why is G41 being used? Tool compensation would have 1/2 the kerf so I would expect to see something like "G41 X0.035" but instead it's "G41 Y12.1304". Had to move the start of the cut to (0,0) to get G41 under control. I doesn't seem to be for tool compensation. Seems like it's being used like G92, the position shift command.

I found this (below) web page, which may be a clue about how G41 is used in postprocessing. I don't understand how the create-profile dialog box corresponds to this. If what I read here is accurate, the kerf of the tool should appear in the arguments for the G41 command---but it doesn't.

https://qcad.org/en/qcad-cam-postprocessor

Looking for any and all input...

neffk wrote: ↑

Sun Apr 25, 2021 7:10 pm

Now, I'm trying to use CAM output from QCAD for a non-test piece.

What QCAM post did you use?

Regards,
CVH

I'm an idiot.

I switched to "G-Code (fofset) [in]" and everything seems to work.

I think the problem was that I changed the settings on the file but not the application preferences.

Hi,
I also have the new Langmuir Pro CNC table, I'm just in the process of learning QCAD before firing it up. I would love to be able to send code directly from QCAD to the Crossfire bypassing sheet cam if practical. How do you workout lead in locations on a drawing? I'm a newbie to all this so I'm wondering if you could help me through the steps to make this happen?

Thanks, Gary.

Garball: please refer also to our QCAD/CAM tutorial at:
https://www.qcad.org/en/tutorial-qcad-cam

Hi again. I knew I wouldn't get far. The instructions for post processors don't match up with what happens on Qcad/cam pro. Either the instructions are incomplete or the version I have doesn't match. For example, when I right click as instructed on a poly line, the drop down menu isn't the same as in the instructions. What am I missing?
My screen shot is attached.
Thanks.

The part you click on is not a polyline (as assumed in the instructions).

You can choose "Auto Create Polyline" from that context menu first to convert your contour into a polyline, then continue as per instructions.

Thanks Andrew. Ok, so I've gone over the instructions and figured out the 'auto create polyline'. I've moved on to creating the 'Cam profile toolpath'. Here in the tool menu, the only available tools are 'mill or drill'. I'm wondering if I've gone down the wrong rabbit hole here as I'm trying to use this for sending output to a plasma table (Langmuir Cross fire Pro). It's never been fired up so this would be the first time.

So I guess my question is: Should I be using 'SheetCAM' instead or is it possible to use the CAM feature in QCAD for this purpose? I'm doing some very basic stuff for now as the learning curve is steep. If I'm going about this wrong, please tell me; I have no idea what I'm doing

I am a complete beginner at CAD/CAM and have spent the last several months learning QCAD. I'm so green i don't have a clue what G code is other than some kind of output for CAM stuff. I really appreciate any 'hand holding' and/or expertise until I can get up to speed then I promise to leave you alone

Garball wrote: ↑

Mon Sep 13, 2021 8:16 pm

Here in the tool menu, the only available tools are 'mill or drill'.

Most G-Code is not tool-aware. You can simply choose "Mill" here. "Mill" for QCAD/CAM means "a tool that can move around in X/Y", unlike a drill. This might be confusing but it can really be a mill, a laser, plasma, glue gun, welding equipment, paper cutter, textile cutter, etc.

There are also post processors that offer a "laser" tool, just for that reason that users might feel more comfortable with that.

Garball wrote: ↑

Mon Sep 13, 2021 8:16 pm

So I guess my question is: Should I be using 'SheetCAM' instead

That choice is entirely up to you.

Garball wrote: ↑

Mon Sep 13, 2021 8:16 pm

or is it possible to use the CAM feature in QCAD for this purpose?

Yes, it's certainly possible and we have many users who use QCAD/CAM with laser or plasma cutters.

Perhaps it's advisable to get a basic understanding of G-Code first and try to run a simple, manually created G-Code file as a first step. This might just take away the fear of G-Code which is straight-forward if you have a basic understanding of the cartesian coordinate system (X/Y axis used for positioning).