I have a task involving a 3/4 inch piece of cherry wood and in the process of creating the piece I want, I remove roughly 0.25 inches from the Z dimension of my piece.
My last operation is to cut the piece in two, so basically taking a piece that is now about 0.5 inches thick and using a contour cut to cut the piece in two although using tabs.
When I set up the operation in fusion it still showed the thickness at 3/4. I set top height as model top and as stock top with neither giving the results I wanted. With model top as âtop heightâ the cutter cut all the way through the material while never creating any tabs. Itâs as if it was going all the way to 3/4 inch deep.
My question is this: Does fusion not account for the fact that the model dimensions change during milling? In this case, the model Z height went from .75 inches to .5 as a result of a face milling operation.
Iâm asking because now it seems I have to âfoolâ fusion to make it think my model is now .5 inches and I would have thought it was smart enough to know, starting with .75 inches and face milling to .5 inches, the model is now only .5 inches thick.
Are you resetting your Z between operations by any chance?
If you set Z (could be the stock top, model bottom, or anywhere else) and your model is 0.5" tall then you should be able to run the facing operation and then, without changing Z, run the contour with a top height of âmodel topâ and have it cut down to the right height. This all, of course, depends on having your Z zero be correct for the stock thickness, etc.
Yes. I do the face mill with a 1/4 end mill and change to 1/8 for the contour cut and I do reset Z to zero in between the two cuts. I have them set so I donât have to change anything (orientation is the same between the two cuts. ) So, I finish the facemill, change to 1/8 end mill, set Z to zero and start the contour.
Iâm kind of baffled.
Having just re-read your post, youâre saying I should set z before the face mill and not set Z before going in to the contour. I see what you are saying but isnât that going to cut through air for the first 1/4 inch?
Iâm ok with cutting air for a 1/4 inch but the bigger problem is I need to shift to a 1/8 end mill for the contour cut, otherwise Iâm cutting too much material away from an already small piece.
What Iâm about to go try is in the contour setup, changing the âstock top offsetâ to -.25 inches. by simulation at least, it looks like it will work.
Are you using a bitsetter, bit zero or just manually setting Z?
With a bitsetter, you can change bits and not change the zero. Setting the top to âstock topâ should avoid the âcutting in airâ by telling it when to start cutting.
Makes sense. In my first post I was assuming a bitsetterâŠ
Have you considered zeroing Z on the wasteboard? I donât have a bit zero, but my understanding is that you could zero x/y using the top of the stock and then Z separately on the wasteboard.
If so, then you could change bits and keep the same zero by just zeroing Z after the bit change As an added bonus, then your stock thickness is less important. If you set the thickness too high, you just get some air cutting during the facing step but you still end up with the right final thickness/tabs.
Can you share the Fusion model?
Typically, you would not model the stock that youâll be removingâŠjust define it as 0.75 in the stock setup. Then, face down to your Model top.
To answer your question: youâre right. Fusion 360 does not, by default, recognize changes in Z dimension. When you set the stock size for your setup, it will remain that size for the whole setup. Same goes for the model.
How to get what you want will depend on your operation:
If youâre using 3D toolpaths, you can set the stock as âfrom previous operationâ and it should skip anything thatâs already been milled.
If youâre using 2D toolpaths, youâll need to go to your âheightsâ tab and change âTop Heightâ to whatever makes sense for your operation.
For example in your case, I donât know what your model looks like but Iâll just say youâve got a 3/4" piece of wood and you want to cut a square out of it thatâs 1/2" high.
To do that, youâd:
Set your stock to 3/4" thick
Set your model as 1/2" thick
Add a facing operation on your model, with âtopâ set as âstock topâ and âbottomâ set as âmodel topâ (or something similar)
Add a 2D contour operation on your model with âtopâ set as âmodel topâ and âbottomâ set as âmodel bottomâ (or stock bottom since theyâre the same)
One other thing to make sure of here is that you do not change your work origin at any point between starting the job and finishing the job. The origin that you set at the start stays for the whole setup.
The bit I think you missed here is setting âbottomâ. The tabs will be relative to the bottom of the cut.
@Moded1952 Basically covered it. It is easier to see what youâre trying to do and where the issue/confusion is when we can see the model.
Hereâs an example with zero set at the top as I pictured the problem youâre describing. Watch the simulation and, as Lucas said, the key is toolpath âHeightsâ tab. Face&Cut.zip (78.0 KB)
Sorry. I wasnât sure if I should upload the fusion file or an image. I think Iâve successfully uploaded the fusion file here. Compress Files.zip (228.9 KB)