Problems Slot Cutting a Spiral

[Anonymous]

I've been trying to get fusion to process a slot cut on a spiral pocket and cannot make it work. 

I made a basic spiral, but even that was a pain. because you cannot directly draw a spiral in a sketch I had to use the coil tool to make a spiral body. I made this above the surface I wanted the cut in. Then I had to sweep along one of the edges of the spiral body to make sure I got a perpendicular cut. This cut I then made into the face of the material. I made the cut the same width of my cutter (in this case 1/8"). Finally I cut away the initial spiral from above the face. (confusing and convoluted.) 

When I try to select the slot operation, then the chain along the bottom of the spiral I get an error of "Invalid Contour(s)" and it refuses to process. I've tried growing the cut to be wider than the cutter slightly, making sure the ends of the spiral are curved so it's not bumping into sharp corners, playing with all the lead in options. I'm thinking the slot tool just doesn't know how to deal with the spiral shape?

the only way I've been able to make it work so far is to make the cut slightly wider than the tool, then use a 2D pocket with it set to a stepover of the tool's width, and a plunge start (or pre-dril, but something without any eased entry) Doing this I can get it to plunge in and cut around. But this seems like a bandaid to a problem more than a solution. Am I missing something with the slot operation?

I attached a screen shot of the feature. Happy to post up whatever else would be helpful. 

[Steinwerks]

If you could export your project as a .F3D file that would be most helpful, and leave in any toolpaths you have tried, even if they are empty, so we can see what changes would be beneficial.

And welcome to the forums!

Also you can embed images directly into your post by using the Photos button on the Post Message bar just above the text field, which is nicer than attaching them.

[Anonymous]

Attached the archive file. I made a mirror of the spiral, so one is .125" wide and the other is .128" wide, then tried a slot and pocket pass on each. All should be in the file. The only one that succeeded was the .128" pocket. 

I haven't messed with speeds/feeds/cut optimization at all, purely was trying to get it to make a tool path. 

Attached screenshot of what the part looks like.

 

[Anonymous]

I will add that if you make the slot .126" wide, just 1 thou over the desired, the pocket method works. And it did work with a profile lead in instead of a plunge. So I'd get my desired result with just a thou over size, which is fine for my end goal. I'm just confused why the slot operation won't work with this feature. 

[Steinwerks]

Well here's your first issue, the slot isn't actually .125" wide, it's .1247" (this actually varies somewhat along the curves):

The pocket method is really due to the CAM not allowing the toolpath to run over itself. One workaround in these instances is to set your stock to leave at a negative value small enough to be filtered out by the post processor, such as -.00001". 2D Contour will do this as well, and adding a Ramp entry to the Linking tab will result in a pretty decent toolpath. In this case since the slot is smaller than the width of the tool, I had to increase the Stock to Leave value out to -.0004":

You can also "cheat" and use an Open Contour with Both Ways selected on the Passes tab:

I am not sure why Slot fails though, even with a smaller tool. That would be something @fonsecr or @jeff.pek may be able to look into.

[Anonymous]

Thanks, those all look like decent options for other work-arounds. 

Weird that the pocket isn't a consistent width. I would have thought it would be when made with a perpendicular sweep, but maybe i'm wrong. That's not really a cam question though. 

I think one of the above methods will get me to where I need in my real project. Likely the open contour trick. I can just pick one edge and end up with a path that is what I originally wanted.