2D boring problem

[Anonymous]

Hello, all.  I'm new to CAD/CAM and extremely new to Fusion 360 (less than a week into the trial).  I picked up .igs files a while back for the grip panels on a 1911 pistol and thought they would make a nice exercise to gain some experience with Fusion 360.  The CAM process has been incredibly staight forward compared to what I've used in the past until I got to the grip screw holes.  I've tried both drilling and boring strategies with no success.  Trying a drilling strategy simply fails with this error message - 

Warning: Selected face not in job model selection!

Warning: No holes to drill.

Not a biggie, as 2D boring would seem to be a better soluition as the holes are actually stepped with a couple of different internal diameters.  However, this results in the strategy boring on the outside diameter of the hole instead of the inside.  Also, if I select more than one circular face in order to bore the stepped features of the hole, the toolpath fails to generate at all.  The error message says that the tool would gouge.

I'm still at the point of not knowing what I don't know.  I'm sure this is something simple, but an help would be appreciate!

Paul

[Laurens-3DTechDraw]

For the drill problem I think the problem you have not selected the body you are machining in the set-up. There is a special box for model.

Also, if it's not a problem with NDA's it might be a good idea to share the part so people can help you on how they would do this part.

[Anonymous]

Thanks, Laurens.  I tried your suggestion for the drilling strategy, but received the same error.  I can't seem to figue out how to send a link from A360 to share here, but did manage to export the file and have attached it here in a format I hope works.

Paul

[Anonymous]

OK, figured out how to copy a link to the actual file.

http://a360.co/1Iy08QA

Paul

[Steinwerks]

Alright, this imported as a collection of faces, and not a solid, so that's one potential issue. Doesn't mean it won't work, just that it's going to be a bit finicky.

In working through the issue, this is a model problem. Since there is no solid to work from, the default in Bore is to select the outside of this particular face, and I don't see a way to reverse the selection. One workaround is use a 2D Contour and set it to Ramp in the Linking tab, and that way you can make sure it's milling on the correct side of the face. 

[HughesTooling]

If you go to the patch workspace and window select all the faces and select Stitch you will end up with one body. Then go back to the CAM workspace edit the set up and select the new body as the model. Now you have a solid body the Bore op will work.

Mark

[HughesTooling]

Something else to try, in the patch workspace create 2 patches to cover the holes, they are not part of the body and are only selected in ops under model to stop the cutter going into the holes,

In ops you don't want the cutter going into the holes select the patches under Model, leave Include Setup Model selected.

Here's the result with the patches selected.

You can select through the patches for the Bore op.

Files attached.

Mark

[Anonymous]

Thanks to everyone for the help.  I knew it was a problem of faces versus solids, but could not, for the life of me, figure out how to change one to the other.  Got hung up on bodies versus components.  Key learning points for me - stictches and patches!!  I gotta say that so far, I'm really liking Fusion360, but the support in the forum is even better!

Paul