Newbie needs help with plasma/waterjet Post Process

[Anonymous]

I keep getting an error: Failed to post intermediate NC data.

Attached is the log.

I am trying to cut out a simple circle.  The simulate works fine, but the post processor fails.

I am build my own plasma cutter with an arduio driver and trying to get gcode.

There must be lots of users out there like me and a video tutorial of creating a circle with may be some text in it would be Fantastic!!

Thank you

John Pipe

[MattWynn · Accepted solution]

The log message 

Error: Waterjet, laser, and plasma cutting toolpath is not supported by the post configuration.

means the post is not configured for the waterjet/laser/plasma cutting (WLPC) operation.

Add this at the top of the post configuration:

capabilities = CAPABILITY_JET;

You can also enable both milling and WLPC with:

capabilities = CAPABILITY_MILLING | CAPABILITY_JET;

See the jet.cps post configuration for more details of special functionality for the jet cutting operations.

We are right now in the pricess of developing user guides for the WLPC operation.

Can you tell us more about the machine you are building?

[Anonymous]

I found jet.cps which has the command "Capabilities = CAPABILITY_JET" included in it, so I selected that and successfuly ran the post processor and got code.

Now, I am using Arduino Uno with a CNC Shield to drive three stepping motors (X,Y&Z).  This uses GRBL code.  I am building a table and gantry to accept my plasma cutter head which will be  driven by the stepper motors.

My next step is to output in GRBL code. so I can send it to the Arduino.

[MattWynn]

in the Post Process dialog, there is a drop down between 'Post Configuration' and the 'open config' button.  With this you can filter what type of posts a shown in the 'post configuration' drop down.  Pick 'Waterjet / Laser / Plasma' to see the WLPC posts.

Give the torchmate, burny and hypertherm a try and see if it is close to what you want.

I took a look at the GRBL site, https://github.com/grbl/grbl.  Since GRBL does not support cutter comp G41/G42, the control will not automatically offset the toolpath for the cutter width.  The next Fusion update will have 'in computer' cutter compensation for WLPC.  So get a post working so you will be ready.

Remember to not put your custom post in the same folder with the generic posts, it changes when Fusion updates.

[MattWynn]

There is a grbl.cps post for milling.

I tried adding the CAPABILITY_JET like I described but there are still some milling related stuff that makes it not work with WLPC.

Let's see if we can get it enhanced to support your plasma.

[Anonymous]

Really appreciate your help with this.

I have discovered all the plasma scripts and run them.  Only the jet actually posts, but the code is incomplete (it is for demo use only).

I looked at the code to try and decipher it, but i am learning. Then I talked to my gcode guru and he said that the code was incomplete.

I found the grbl post processor and replaced the capabilities line and it failed too. I looked in the rest of the program

to see where that statement was used and could not find any thing and gave up.  So your proffessional help would be great.

I am hoping an update will solve these problems.

Where do you want me to post messages in the future?

John Pipe

[Anonymous]

This is what I am using bought from Ebay.

The link below has a software set up.

http://www.ebay.com/itm/Arduino-CNC-V3-Shield-for-Mill-Router-Engraver-Robot-4x-DRV8825-UNO-R3-/1217...

I don't know it this will help.

John

[skidsolo]

I made the relevent changes to get GRBL to do laser tool paths in fusion, please check this out and give me feedback for anymore alterations you need.

[Anonymous]

It is trying to work, I still got an error though, see attachment

John

[MattWynn]

change to 'in computer' compensation insread of 'in control'.  It may give you an error when you create the toolpath (since 'in computer' does not work yet), but you should get a toolpath that will go through the post.

In computer compensation for WLPC is in the September Fusion update.

[Anonymous]

That posted, yes!

[Anonymous]

Adding to my previous post.

That should ba a big YES!!     "WE HAVE LIFT OFF"

Not only did it post from Fusion.

I somewhat understood what the code was doing and i verified it with  simulation on grbl sender.Then I loaded the code on to the arduino, although I don't have stepper motors connected, I could see the led flashing.The position co ordinates on the sender were doing the right thing and I got lots of green dots (thats good succesful comands).

VERY COOL

Thanks a bunch

[MattWynn]

Very happy, great news late on a Friday.

Let us know if you have other success or failure.

[skidsolo]

Very cool and exciting !

Sent from Outlook<>

[Anonymous]

I'm on a roller coaster here.

Post worked for a rectangular cut, although it went down then back up and around.

But I get an error for a circular cut, see attached log.

John

[MattWynn]

The message :

Error: Radius compensation mode not supported by Grbl.

 is because it seems the grbl does not support cutter radius compensation in the control. (Yes, same issue as smoothie.)

The September update will have in computer cutter compensation for WLPC.  You can still select 'in computer' compensation on the passes tab: you will have a warning on the toolpath and the the part will be cut undersize by 1/2 the kerf width.

That should get you back in business!

[MattWynn]

And you can remove the up down moves by setting the retract and clearance offsets to 0.  But be careful : if parts tip after being cut and you move over them you would crash the head.

[Anonymous]

I am afraid I am out of my depth.  As I understand, there is no milling cutter involved, just a plasma stream or water stream doing the cutting, agreed this does have a kerf .  I don't expect ultimate accuracy from a home made plasma cutter. I will be happy just to make it work.

When can we expect the September update?

Regards

John

[Anonymous]

I have been quietly working on my home built plasma cutter and wanted to report in.

Since this last software release, I have got it working.  I can make a sketch or load a dxf shape and cut it out.

I sucessfuly use the jet cps (which works despite being demo only) and modify the turn on/off plasma code with Notepad. I am using the "coolant on/off" output to trigger the plasma cutter.

Thank for your help.

John P

[MattWynn]

That is great news John, thanks for checking in.

When you get to the point that you are always making the same edits to the code, let us know and we can modify the post so you do not have to make edits.

Do you have any pictures to share?  Or post a project on the gallery!  I love pictures.