Plasma Cutting using Multi axis?

[bucksanimals200hd]

Hello, I have a plasma cutter strapped to a fanuc robot, and want to create a system to cut two simple holes in a piece of angle. However, it doesn't appear that it is possible to do that with fusions limitations. I tried to use a milling bit to replace it, but I got the error "no passes to link" and I got no toolpath created. I also don't know how to make there be no stock attached. Any help would be greatly appreciated!

link:

https://a360.co/3zIJhtx

[alexandre.pintoAGNAU]

Hi @bucksanimals200hd 

At the moment FANUC Robot post is still to be released, it has been tested with success but just not enough as we require to release. So we do not have documentation or a link for this yet. Attached the post enabled for "fabrication " toolpaths as well as additive and subtractive.

I would say the first thing you need to do is read through the KUKA and ABB pdf guides we made available.
https://cam.autodesk.com/hsmposts?p=abb
https://cam.autodesk.com/hsmposts?p=kuka

This will explain Tool setup in detail, Fusion 360 posts only support tool with Z+ up and Z+ down. And you need to define the tool on your robot with one of these 2 configurations. Then make sure you pick the correct option in the post.

I recommend you find a way to measure a User Frame by 3 points on the robot, preferably using a calibrated spike. 
You will need to replicate the User Frame in your setup in Fusion 360 setup (example below).

The setup you have in your project means measuring X axis on the robot would be hard as X axis is in the air, so below I measure X axis along a Edge and XY plane on the beam. I hope this makes sense.
P1 is origin
P2 is along X axis
P3 will be the XY plane

Once you have figured out the correct setup and post configurations you are good to go. I highly recommend an air move high above the part first to validate what you have done.
You can then run a job right on the part without laser ON/OFF.

Once you are happy with what you are doing update the post so that the ON/OFF code is correct for activating your external device via the FANUC I/O.

Below you can see a sample output (this sample is ASCII format, FANUC uses Binary!! so you must have the ASCII upload option  to convert and run the file on  your FANUC robot).

 Search the post for this code, and replace with whatever you are using.
 

I believe this is everything you need to cut your part on the FANUC.

Regarding Milling toolpaths.
I created a setup where I define the workplane on the corner as specified before.
I also defined the stock as a model and that means "no stock" as you want.

Created two 2D Contour toolpaths, one aligned to the Z of the setup workplane, in the second I changed the workplane and it cuts the side hole also (see toolpath options).
Take care with connection moves, or run a toolpath per setup and have different user frames so you work safely in one orientation/setup at a time if you need.

Good luck and keep us posted.

[alexandre.pintoAGNAU]

Also interesting is to read up on this post.

https://forums.autodesk.com/t5/fusion-360-support/ur-robot-post-processor-plasma-fail/m-p/10418678

[bucksanimals200hd]

That almost worked, I am actually using robodk software to run the robot and importing the fusion toolpath. When I import what you gave me, because it is 2d contours, they are loading in flat, and not aligned to the piece, as the setup origin is what is used to place it by a reference frame in robodk. I believe I need to be able to have the toolpath relative to the origin. I attempted to use an end mill to use my trial of the machining extension, but I could not offset the toolpath above the piece to account for the plasma cutter.

Thank you,

Jeremiah

[alexandre.pintoAGNAU]

Hi Jeremiah,

Have you NOT succeeded with loading and running a job without Robot DK, directly from Fusion 360?

Have you tried ?

I am not a Robot DK user so I cannot comment.
But I would say that positioning a part and then running a job relative to a coordinate system on the part should be possible. 


Alex