[rccars4sal]

Hello all. Im trying to use fusion 360 because my old bobcad died, and it is not supported any more. Yay me. So, I have a library of hundreds of CLEAN dxf files that I need to sometimes edit. Simple things like rotate the drawing to fit a work piece material or lengthen a section. No big deal. I have been trying to generate g code, but the fusion just keeps saying tool path not supported by the selected tool. These are simple 2d drawings where the tool path is just entry, plunge, cut, raise, exit, stop. I just want to make simple tool path and g code. Is it wrong to select 1/8" flat endmill for a simple profile outline? The file in question is a simple outline about 12" long and 7" wide, with some radiused corners, and all radii are large enough that a 1/8" endmill is and has been fine.

I know what some of the issue is. Fusion wants to calculate offsets, feeds and speeds, and it thinks I am wrong. All of that is stupid. My drawings are such that tool offset is calculated into the line work. I edit feeds and speeds for every run because I use different materials, wood, carbon fiber, fiberglass, delrin, nylon.

Can somebody please help me to get this working? My business is on hold because I no longer have a cad cam solution that works.

Ive also been trying stand alone cad and gcode generators. Now thats really futile.

[Jim Dawson]

I have been trying to generate g code, but the fusion just keeps saying tool path not supported by the selected tool. Is it wrong to select 1/8" flat endmill for a simple profile outline?

I know what some of the issue is. Fusion wants to calculate offsets, feeds and speeds, and it thinks I am wrong. All of that is stupid.

My drawings are such that tool offset is calculated into the line work. I edit feeds and speeds for every run because I use different materials, wood, carbon fiber, fiberglass, delrin, nylon.
.

I would have to see one of the drawings that this error is occuring on. Export a F3D file, zip it and attach it to a post.

Calculating feeds and speeds is what Fusion kind of does, but Edit the Tool to make adjustments

If you have already done the tool offsets in the DXF file, then use the Trace operation to do the part. It cuts exactly where the line is.

I should note here that Fusion CAM wants to see a 3D part, not a 2D line drawing. Try extruding the part you are working on, then run it through the CAM function.

[peteeng]

Hi RC & Jim - I use trace quite a bit for engraving and it works very well. But RC you will need to learn how to use Fusion more efficiently or any other CAM program for that matter. Fusion will work from solids or sketch's. If you try to force a CAD/CAM system to work the way you want it to work you will just become frustrated. Learn how the system operates and your life will be easier. Fusion does not calculate feeds and speeds you specify those. It will pick default values but they can be changed at any time. Tool side 0ffsets can be spec'd by you as well. Fusion places a small pointer on one side of the line and you can pick that and change the side. Trace places the TCP on the line. Its best practice not to include the tool offset in the toolpath and let the software calculate that for you. Then things like tool wear and spring back can be included into the toolpath or if you change the tool dia it updates the path automatically. I'm sure with a little practice you will get how Fusion works, it works the same as any modern CAM system does. If you are going fwd with Fusion I would import a dxf, offset that to the correct geometry and then go fwd with the correct geometry vs an offset toolpath file. Then you can take advantage of Fusions features. Currently you are very limited by using geometry or sketches that include the offset. Peter

edit - one issue you may be having is the chaining tolerance. Depending on a few things in the native CAD you created the dxf with, means that the imported lines may not be connected or connectable or contiguous. This means when the CAM side tries to chain the geometry together it can't so you may have to select each bit of the sketch individually or go back to your CAD and export the dxf at a higher tolerance so the chaining works properly. Or go into Fusion CAD and join them together... learning curves are always tough but you do come out better off. I'd say you will be better off using Fusion then your last system once you learn how to use it. The penny will drop when you relax...

[peteeng]

HI RC - I played a little with Fusion and can't get it to respond with an error in the form of " tool path not supported by the selected tool" using trace or profiles. The only time I have seem that sort of error is if you are selecting "V engrave" then it is expecting a tapered bit. If you select a flat or round bit it will tell you the tool is not suitable for v engraving - fair enough. Is this what you are doing? see attached image of error. Peter