Post Processor Help

[kmcgheeCMFPG]

I am using the standard Torchmate 3 Post Processor with fusion for my plasma table. When I load the code into the torchmate I get a few errors, if I remove the lines of code that are causing the error it works fine. So I need some help learning how to edit the post. I have attached three posted files for a simple 1/4" thick 6"x6" rectangle.

The first is generated by RhinoCam and what I have been using for years. The second if the code generated by Fusion that gives the errors, the third is the fusion file with the deleted code that cuts the part out just fine.

I did have to disable the useZ property to get rid of fusion trying to control the Z height.

Can anyone direct me in the right way to edit the post to output the desired code with the problem lines eliminated. I also would like to know how to add a line of code so the machine returns to 0,0 when its done cutting the part. 

I have put in three pictures of the errors that come up do you can see just what was going on. Note that it shows two errors for line 6, I deleted line 6 which then reset all the lines, and line 7, also causing an error, was renamed line 6.

[kmcgheeCMFPG]

Anyone? I have an entire class of students getting me to individually edit their code, its wearing thin.....

[Steinwerks]

I will try and look at this tomorrow. Which post processor are you using?

It looks like you only need the work offset removed (G54 line) and the homing move removed (G28). You should be able to turn off the M8 in the tool but I almost never touch the laser/plasma/waterjet stuff so I'll have a look at that.

[kmcgheeCMFPG]

I am using the torchmate.cps - Torchmate 3.o Mill/Plasma post. I think if you were able to make the post remove those lines and possible not post out M codes, I cannot seem to find anywhere in the toolpath or tool itself to turn off the M8, or tool change so I need that to go away too. If I could understand the post I would tryt it myself, in fact I have and I am a terrible programmer.

[Steinwerks]

Your post appears to be different than the default one installed with Fusion 360. Can you attach it here? This is the code I get for a simple square:

(test)
N10 G70
N11 G90 G17
N12 G28 G91 Z0.
N13 G90

(2D Profile1)
N14 M6 T1
N15 G54
N16 M8
N18 G0 G43 X1.2098 Y0.9639 Z0.6 H5
N20 Z0.
N21 M50
N22 G1 X1.1902 Y0.998 F39.37
N23 G41 D1
N24 X1.0197 Y0.8996
N25 X1.0026 Y0.8897
N26 X1. Y0.8852
N27 Y-1.
N28 X-1.
N29 Y1.
N30 X1.
N31 Y0.8655
N32 Y0.8458
N33 X1.0026 Y0.8412
N34 X1.1902 Y0.733
N35 X1.2098 Y0.7671
N36 M51
N37 G0 Z0.6

N39 G28 G91 Z0.
N40 G90
N41 G28
N42 M30

[kmcgheeCMFPG]

I am using the one that installed with Fusion. There is at least one difference, in the program settings I have told it to ignore useZ. I also when using the post have it selected to cutting. though it appears to not make a difference.

Post attached.

Thanks so much for helping!!

[kmcgheeCMFPG]

Oh here is the test square I used to generate that code.

[Steinwerks]

Try this post. As usual with any edited post, test with extreme caution.

Oddly enough the post skips the block numbers even though the writeBlock function has been disabled for coolant and the work coordinate block. I am not sure why it keeps counting.

@jeff.pek Any idea why coolant is enabled here? Or why it exists in the Torchmate post? It appears to be in the tool definition (dump.cps outputs tool.coolant=1) but there's no way to change that as far as I can tell.

[kmcgheeCMFPG]

Thanks, later today I will be going to work and will test it out, hopefully it will not require any more edits. I appreciate the time you have put in helping me, my students will be greatly appreciative. Time is running out in the semester and many are trying to cram in lots of plasma table art before school ends.

[AchimN]

It seems that the latest post on the post library has properties for all the changes you would need.

The post is available here:

http://cam.autodesk.com/posts/?p=torchmate

We will look into the problem that coolant is active by default.

[fonsecr]

Opened CAM-7728 for coolant issue.

[kmcgheeCMFPG]

First and foremost I want to thank each and every one of you for your help, this new post, works great. I know have the control I need to run my students files. 

Is is possible for one last bit of help; is it possible to have the post changed so that when the file is complete, after the plasma off, the machine returns to X0, Y0? All my CAD and Plasma tutorials work off the premise that the machine will return to o,o and it will cause major confusion from these teenagers if it doesn't and I would really not like to edit hours and hours of videos and documents.

Thanks!!

[Steinwerks]

Do you want the previous one I shared to do so, or the one found on cam.autodesk.com?

[kmcgheeCMFPG]

The one from cam.autodesk.com worked perfectly, that one please!!!!

[Steinwerks · Accepted solution]

Here's the output from your test post. I just made a new user variable in the dialogue called returnXY0 that is enabled by default.

(Test)
N10 G70
N11 G90

(2D Profile1)
N12 M6 T1
N13 M8
N15 G0 X5.9375 Y6.1875
N17 M50
N18 G1 Y6.125 F86.
N19 G3 X6. Y6.0625 I0.0625 J0.
N20 G2 X6.0625 Y6. I0. J-0.0625
N21 G1 Y0.
N22 G2 X6. Y-0.0625 I-0.0625 J0.
N23 G1 X0.
N24 G2 X-0.0625 Y0. I0. J0.0625
N25 G1 Y6.
N26 G2 X0. Y6.0625 I0.0625 J0.
N27 G1 X6.
N28 G3 X6.0625 Y6.125 I0. J0.0625
N29 M51

N31 G0 X0. Y0.
N32 M30

The silly coolant code is still in there however.

Edit: because I had useCoolant set to Yes. Oops.

[kmcgheeCMFPG]

You guys are awesome at autodesk. Thanks so much.