I’m confused about the WCS Setup when I’m using bitzero. Does the below look correct?
Suppose I’m using Bitzero to probe the lower left corner, top of the stock material. Would I then in the Fusion 360 CAM setup orient the stock the way it would appear when viewed from the front of the machine, pick the origin to be the bottom left corner, top surface of the stock, with the X axis increasing to the right, Y axis increasing away from me, and Z axis increasing up? This means when actually milling it would be driving Z negative, but I guess this is OK because it knows it’s starting at the top surface?
Suppose I now wanted to do some milling on what was the bottom surface so I flip the board front to back, so the bottom left top surface is now the top left bottom surface. In case I don’t have my stock X&Y dimensions measured exactly, I suppose I would now want to measure the same corner, which is now the top-left corner, but probably the (newly) top surface still since the depth should be good to a fraction of a millimeter. So in CM I would now tell it that I was using bitzero on the top left corner, top surface. In Fusion I would re-orient the view to the way it would look of viewing it from the front of the machine, move the Origin to the top left, top surface of the stock, and again set the axes up to increase the same way the machine does (X increasing to the right, Y increasing away from the front, Z increasing above the stock surface).
Sounds right to me, but my recommendation has always been to make a pair of simple test projects, one in Carbide Create, the other in whatever 3rd party software you are trying to set up, then run the Carbide Create file and export it to G-code, then compare the 3rd party software’s G-code — if things match up (consider using a 3rd party G-code previewer), then try the file.
Yes, your zero setting sounds correct, cutting with Z < 0 is fine if you’re cutting below the workpiece zero.
I generally use the bottom of the stock as zero, that way I don’t have to ensure that the thickness is exact and consistent and I plow into the spoilboard less often. Here’s a recent machining setup, Front Left SpoilBoard Zero with a manually selected Z axis plane & X axis to set the X, Y, Z directions and then the front, left, bottom corner of the stock solid selected as workpiece zero.
Regarding flipping and machining the other side, search the forums and there’s plenty of threads on flipping and machining, there’s a few things to be aware of and I’d definitely try a simple part first on some cheap material as you’ll likely mess up at least once.
Where I need a really good alignment I tend to use a fixture plate (some old MDF) which I work from the front left corner of as an overall zero. I then bore some 6 or 8mm holes in the fixture plate using the Shapeoko, these are for dowel pins to align the stock.
I then bore matching holes through the stock, again using the Shapeoko, and then mount the stock on the fixture plate using the pins. I machine that side using the zero from the fixture.
I then flip the workpiece, onto the same pins, using the other side of the holes bored through the stock, this gives a consistent flip orientation.
I tend to use the fixture surface (bottom of stock) as Z zero to avoid stacking up errors there.
When you flip the stock you need to ensure that
The flip is exact about X or Y axis, however you align the stock, that X or Y edge must be consistent when flipped or your two faces machine at an angle from each other
The X, Y zero when you flip is consistent, you can do this either by the method you suggest, re-zero-ing off the same corner once flipped, or through precision in measuring the stock before the job, or though using a fixture and boring alignment holes
The Z dimension and zeros line up after the flip, if there’s any difference between the Z dimension of the stock and the CAD model this error will double when you flip if you’re zeroing off the top of the stock
Thank you very much for the detailed information - you have saved me a lot of head scratching! (e.g., Measuring Z from the spoilboard is smart!).
How do you align the fixture plate with the machine X or Y axis. I was thinking that (precisely) drilling some holes through it and into the washboard and then using delrin pins or similar for alignment might be good (people sometimes do this with Shaper Origin), and I’v ealso seen videos from C3D where 1-2-3 blocks are used to offset from a piece of wood machined to be parallel to the Y axis in the left-most T-track.
NP, happy to help, there’s a lot to figure out and the community here is great at helping us get started.
I have three approaches to aligning the fixture plate, depending on the job
Using it once, I just bolt it down to my spoilboard reasonably square (I hid m6 tee nuts underneath my top layer on my old SO3), on the SO5 that probably means bolting down to the T slots and then machine the dowel pin holes and don’t move it until the job is done
Using this fixture more than once, but not many times, I bolt the fixture down to the spoilboard, then I stick a dial indicator into my spindle and tram the X axis edge of the fixture straight with the machine, tighten, bore holes etc. This way I can re-tram the fixture plate for a second or third job
Using this fixture plate lots of times, as you say, bore some locating pin holes into the spoilboard and then bore holes with matching offset into the fixture plate, pin it to the spoiboard and then bolt it down.
I have found that I get a surprising number of re-uses out of each chunk of MDF I use as a fixture before it’s such a swiss cheese I throw it away. Also, it can be handy to soak a little CA glue into the reference corner of the fixture MDF to harden it up and keep that corner consistent, I also do this on frequent use down pin holes. Soaking in a little CA, setting it with the activator and then running a machinining finish pass on the edge or bore gives a nice solid face which takes much longer to go all fluffy.
