How to create offsets for complex patterns?

[mrburnsns]

I need to create offsets to take into account the kerf width of a laser cutting process and the need for several passes around the same path.   The application is for a resistance heating element that will be laser cut (example attached), so the path is very complex.   I first tried a basic offset of the DXF, but Offset wasn't working (it just gives an error without further explanation).   I then tried to create surfaces in the Patch environment, which worked, but seems to have stopped working when I tried to fix an error in the file I created a few weeks ago (Fusion just locks up or gives an error).   Does anyone have any strategies that I can try short of manually offsetting every curve (the example shown below is a very small section of a much larger element)?   I need to export the path as a DXF, so I don't think I can use the CAM milling features.

[Anonymous]

Mind attaching your DXF or F3D file?

[TrippyLighting]

I would actually not use a XF file just to avoid the typical problems that that been reported here with DXF files.

Sketch the center line of the laser path using the sketch tools in Fusion 360. That'll unfortunately a bit off work.

Extrude this with the extrude command in the patch workspace.

Thicken that surface to the kerf width of the laser.

Create a solid with the outline of the base shape and extrude it.

Combine/cut the thickened meander surface from the plate.

See  the timeline of the attached file for the workflow.

[mrburnsns]

I can't send the original files, but here's a cut down version of a file that demonstrates similar issues.   It shows as a closed loop in 360, but Fusion balks at offsetting the curve.  This file allows me to extrude the solid, then offset from the edge, but it doesn't see the "loop" that the extrude function does for some reason (so I have to select some faces  on the side of the path manually in the patch environment).

[mrburnsns]

I was figuring the DXF might be causing the issues - interestingly if I cut the path into smaller sections, I am able to offset.   Are there any "tricks" people have discovered to clean up DXFs?

Interestingly I have a few files in DWG format, and they have the same issues...  

In any case, thanks very much for the video.   I was thinking that's where I was going to end up, but there's a few tricks in there that will be helpful if it comes to that.

[blub19 · Accepted solution]

how about extruding the part you want and then using CAM with the cutting option and autdesk dxf export to produce a correctly offset dxf? That's how I create dxf for my laser.

[TrippyLighting]

Could you create a screencast and demonstrate how that works ?

This sound like a nice workflow to have in one's tool box!

[mrburnsns]

Gonna give that a shot now - wasn't thinking that's an option, but if it is I should be able to create three DXFs and export them as layers to my marking software.   Thanks!

[chrisplyler]

I've never done any CNC myself. But I was under the impression that most CNC software used on things like laser cutters or water jet cutters have the ability to adjust for kerf width built in. No?

[mrburnsns]

Yep that seems to work - I had to use the 2d Contour option for some of the more complex patterns (with the laser being a "very small mill"), but I generated the paths.

I had to download a post-processor from Autocad's site here: https://cam.autodesk.com/hsmposts?p=dxf

It's also necessary to disable In Control compensation before generating the toolpath or the post-processing will fail.

Once I did that, I just right clicked the toolpath in the browser, selected post-process and I was off to the races.

[mrburnsns]

Unfortunately no pathway compensation on the budget unit/software being used. On higher end units, yes absolutely that's the way to go.

[chrisplyler]

@mrburnsns

Gotcha. I'm wondering if you can set up a tool diameter in Fusion's CAM workspace that equals your kerf width, set up lead-in distance so your pierce would be away from the desired edge, and then generate code without all the rpm nonsense that a laser cutter wouldn't need. Can you tell from my idea that I haven't ever done any CAM work? Any thoughts?