How to make a clean profile cut

I’m using Fusion360 with the x-carve to cut profiles in plywood. The measured thickness of the ply is 5.1mm so I draw the model using this thickness. I then configure CAM (in Fusion360) to cut the profile. It does this but cuts 5.1mm deep which with manufacturing variance in the material, doesn’t always cut right the way through and leaves a ragged edge on the underside. How can I tell Fusion to cut a little bit deeper so that it goes through the material into the sacrificial board underneath? I’d like to cut say 5.3mm deep through the 5.1mm material.

If its only profiles you’re cutting and not pockets, you can add 0.2mm of stock offset on the top of your stock. You can do this in the Setup of your CAM operations.

Not sure with fusion360, but when I do this, i set the depth of cut slightly deeper than the material thickness. So if the ply is 5mm, I’ll cut 5.5mm (1/2mm deeper).

Be aware that this will cut into your table, so you’ll either need to have a sacrificial table surface or you need some waste board under the work.

I guess there’s another couple of options such as setting the Z Zero a little too low, or setting the work thickness a little too thin, but I’d prefer setting everything accurately, and then purposely cutting through the bottom of the job.

Not sure if fusion360 warns you or not, but VCarve Pro provides a warning when cutting through the bottom of the work, so this is a nice double check/reminder that I’m actually doing what I’d intended.

Hope this helps a little

Just go to your “material left” option, like you’d use for leaving an allowance for a finishing cut, and put in a negative axial value. Like “-.020” will cut down to .020 below your material, if I’m recalling correctly. I’ve used that to adjust the size of features on an imported STEP file that I can’t change properly before. I’ve only used a negative radial offset, though… Probably will work in axial as well, although it might throw a cut-through warning? Not sure.

@DanBrown that works just fine, thanks.

Cool, good to know! Hadn’t actually tried an axial over-cut like that myself, but I’m going to be adding that to the bag of tricks now. :smile:

I do this backwards from the way you’re going.

Create your design using a number you pick for the material size - say, 5mm. Don’t worry (yet) about your actual material size.

When you go to CAM, do some things different than what you’re trying:

• Set the axis indicator to the bottom of your design, not the top.
• Set your Z-0 for your workspace to your wasteboard, not the top of your material. You can add a touch of fudgefactor here to cut slightly into your wasteboard if you want.
• In the stock pane of Fusion360, set the actual measured width of the material you’re cutting, and go ahead and add a bit of a fudge factor since the width of plywood isn’t all that consistent.

It might a little bit of aircutting (depending on your fudge factor), but this will cut all the way down to the wasteboard and IMHO it’s much easier to set up.