Post processor for ESAB plasmacutter with vision 2000 control

[Anonymous]

Hello

I cant seem to find a post processor to make dxf files for our ESAB plasmacutter with vision 2000 control.

Does it exist?

Best regards

Morten Lund

[Tom.Hemans]

Hi @Anonymous,

If you cannot find a post on the forums, you can try searching through the Post Library for a similar plasma post that might work with your machine. Or you can contact one of our CAM partners via the Service Marketplace who can provide a post for your specific machine.

Tom

[Anonymous]

Were you able to find a post for this machine? I have the same control on a waterjet and was hoping to have a reference for making/editing a post.

Thanks,

Chancellor

[Anonymous]

Sorry, I didnt have any luck.

I have used IGEMS software to create cutting files (which is originally developed for waterjet cutting I think).

Please let me know if you have any succes, thank you.

Best regards

Morten Lund

[kyle.kershaw]

Hi @Anonymous and @Anonymous 

Nesting in Fusion360 is coming out soon. With that said, Autodesk would like to be able to support as many laser/plasma/waterjet machines as possible. I'm a post guy and would love to make Fusion support the ESAB lineup. 

Here's the proposition. Send me a working NC program (or programs), along with something that describes the shape it's cutting (ideally a Fusion .f3d file but can be a drawing) and I'll see if I can't reverse engineer a post out of it. Any machine specific documentation would also be helpful. Attach them here or send them to me in a Private Message and I'll see if I can't make a post to cut your parts.

If anyone else reading this wants to play, feel free to send me your info too.

ps, there are two "dxf" posts in the Post Library.  Don't know if you've seen them or how appropriate they are but I thought I'd mention it.

AutoCAD DXF

Universal Laser DXF

[Anonymous]

Kyle,

I am in the same boat. I have a esab vision 51 that I am currently trying to program but cannot find a post processor for it. 

Please let me know if you can help.

[kyle.kershaw]

Hi @Anonymous 

There is no ESAB post right now. That's the reason you can't find one.

Can we make one? Depends.......

What kind of file does the ESAB read and actually run on? The first entry in the thread talks about using a DXF file. I assume the DXF is translated into something the machine reads and runs on. Do you know if the ESAB "converts" a DXF file to NC code and then runs that? If so, can the "converted" file be saved out?

If so, I'd like to skip the DXF step and go directly to G&M code (if he machine can read G&M code). 

Can you send a working program that the DXF creates (and that the machine reads and acts on)? That, and a description of the shape it's cutting, and I'll see if I can't reverse engineer a post out of it.

Again, there currently is no ESAB post. But, if you can show me the code the machine reads and runs on, there is a possibility I can create one. Do you know what code is created from a DXF?

[Anonymous]

Kyle,

The Esab with the Vision 51 controller uses EIA format. The file types it accepts are .mpg and .cnc I believe. 

Attached is the Esab programming manual, that is all the resources that I have right now.

Thank you

[Anonymous]

@Anonymous I was able to write one that worked for our machine and am willing to provide it, but it would be "as is" as I am not certain it will work on other machines. If I remember correctly it outputs to ".cnc" format. I do not write posts for a living, I just get lucky from time to time! If you would like a copy of it please let me know, again I am assuming no liability as to how this would work on your machine.

[kyle.kershaw]

@Anonymous Thanks for the manual. Helps a ton.

@Anonymous I'd like a copy of that post. If you would, please send it to me via private message and I'll review/enhance/bless it into existence for the rest of us. (liability exception accepted)

Thanks

[Anonymous]

@kyle.kershaw Sounds good! I'll try and get it your way later today as it is not on my current work computer.

[kyle.kershaw]

FYI @Anonymous @Anonymous @Anonymous 

I talked with an applications guy at ESAB and he told me the current programming manual is the F-14-082 that Schu5888 atteched previously. I'll use that to make a post and hit you guys up to test it.

Stay tuned.......

[kyle.kershaw]

@Anonymous @Anonymous @Anonymous 

Hi Guys

The ESAB Plasma post is ready for review. Private Message me if you're interested in testing/critiquing/using the new post and I'll send you a link.

[kyle.kershaw]

@arni @ckurre @Schu5888 

Any interest in ESAB plasma post testing? 

M65/M66  plasma on/off. M67/M68/M69  comp left/right/off.

Private Message me if so.

[Anonymous]

Kyle,

I got my machine up and cutting. I will be testing out the ESAB post today.

-Matt

[kyle.kershaw]

Hello All

@Anonymous , @Anonymous , @Anonymous , @Anonymous 

An ESAB plasma post is available for beta testing. It's not on the main posts page (https://cam.autodesk.com/hsmposts) but can be found here.

Give it a try and let us know how it performs!

[Anonymous]

My tech guy told me, as long as auxiliary function are match there'll be no issue on our daily use but unfortunately he can assist only with ESSI format as per his expertise, if this post processor can produce EIA and ESSI format would be great

[ASagalajev92]

Hi , 

I will test that on our ESAB plasma and let You know how it goes... Tnx lot for Your work !

[perW789Z]

Hi all!

Came across this forum thread as i was searching for a postprocessor to output ESSI format from Fusion 360 for use in an old ESAB NC 510 control. I have altered and attached a post that works fine for us and want to share it, if anyone  have the same challenge or need. It is set up for Oxyflame cutting. Jetmode/watercutting must be chosen in F360.

IMPORTANT: ALL VALUES MUST BE POSITIVE for this post to work! Action must be taken to place part including IJ cc points on positive side in XY plane in F360 prior to post processing or else output will be corrupt. (This is a result of my limited skills in javascript programming  and a lack of solution to a problem concerning ability of post to treat and output the «+» sign on postive values)

Absolute IJ must be marked on (= in use) in post properties.

Circular interpolation must be marked on (= not in use) to get smooth curve movement. If part only have very large radiuses this can be marked off (no mark= in use) as this eliminates cc points on negative side.

Rapid start/stop=5 and 6. Cutprocess start/stop 7 and 8. Left comp 29, Right comp 30, No comp 38, End program 63, Absolute coordinate 81. No feed and height output as this is external on our machine

Enjoy!

[tholmesCC6G3]

Where are we at on all this? I have Inventor CAM and a ESAB 1000 that needs a .mpg program. What .cps file do I need, It will be as simple as this.

M68
G0X5.179Y-1.306
M70
G1X6.262Y0.088
G3X6.462Y0.195I6.258J0.338
G1X7.538Y1.731
G3X6.104Y2.734I6.821J2.233
G1X5.341Y1.645
G2X5.073Y1.546I5.136J1.788
G1X1.565Y2.460
G3X1.272Y0.000I1.250J1.250
G1X6.262Y0.088
G1X7.345Y-1.306
M73
M69
M71
G0X0Y0