I am practicing with a simple part, but doing (2) ops, requiring a part flip. I am trying to mill the contour approx 70% depth on op1 leaving a “hat” and then removing the hat and taking remaining 30% contour on OP2. The drilled hole is my WCS for both ops.
This is to simulate a tall (Z) part where I can’t do it all in one pass with shorter end mills.
I keep getting this gauging on the finished face of OP1 as you can see in the picture.
Is this unrealistic ? Can the MR1 hold this tight of tolerance to have a seamless profile match after flipping part? Its a very small ridge..but still, its there.
Everything has been trammed to .0005” on the machine. I am a bit of a perfectionist in that regard so been shimming and measuring for a week! Thanks
You can definitely get less mismatch than that on the mr1. Using the probe? Edge finder? I find the probe does really well finding the center of holes as long as it’s dialed in really well. You sure it’s not your set up?
Edit: it looks like the short side has way less mismatch than the long side…
You can get it down to a much less visible blend line in the cuts. The main things are if your X,Y, and Z are pretty square, and getting a good offset from that hole. I usually use a dial indicator and manually get my offsets for flip over operations. The probe, for me, hasn’t been accurate enough to avoid having a little step on the 2nd operation.
hopefully i can help you, i had this same issue when milling wood blanks on my shapeoko for hand guards on a revolver. you need to square your stock, so imagine you have your model in the middle of a 2x2 piece of material. on the program it thinks its 2x2 but you may have a piece that on 1 axis (lets say X) that is 2.1 well if you mill the top and flip it over to mill the bottom your part will be off by .1 as you are indicating off of 1 side. if the material is off by a small amount and you have more finishing to do or you dont care to much about small offsets (much easier to say about wood stuff than metal) you can indicate of one side the offset to the middle. so touch off on X and if the material is 2.1 go to 1.05 which would be center and the offset will be minimal or non existent.
This is probably the most difficult thing to do on the MR1. I’ve failed to do it perfectly a number of times and have largely just used longer/larger tooling that makes it a non-issue.
The spindle is repeatable enough. Using the Langmuir probe, I haven’t done bore probing GR&R but wall probing is repeatable for me to within about 0.001”.
Fixturing is your most likely culprit. I get much better repeatability on a y facing wall vs an x facing wall. The y facing wall is hard datumed against the vise. The x facing wall can be tilted (even if the parallels are clamped, that only tells you one edge is clamped against them). If everything is not perfectly square to the first side, you’ll notice in the output cut.
Even though you are probing on the bore, if the 2nd side fixturing isn’t square, the walls you are actually machining will still have tilt and show this issue.
Some have opted for the Heimer 3D Probe since you can use it not only for probing but also for checking squareness and fixturing. Because it’s a calibrated mechanical probe, you know there’s no funny business going on.
If I were to try harder down this road, I’d probably get the Heimer and start studying the repeatability of my fixturing/part flips.
so what do you indicate off of for the hole op? because if your stock isnt squared and you run the hole op it wont matter if you indicate off your hole because your hole will be off.
Can you get better than that? Probably but it’s a pain in the a**. I just use stock that is 3/16” to 1/4” thicker and do everything from one side. Than flip it over and mill off the extra. Perfect part every time.
You don’t have to machine all sides square, but op 2 should only ever datum to things you’ve already machined and even then, you have to work hard to make sure the machined faces from op1 are square with respect to the machine.
design it as a two piece assembly that bolts together. You can design anything but if it can’t be made than you’ve failed. When customers ask me to make parts for them I always offer to “help them modify the design so it can be produced more economically” (aka on the MR-1). If they refuse design changes than I give them a stupid high price and send it off to be made at a local shop that has a $100k VMC. I pass it through and take my cut.
Most machine shops I know work with each other like this. Not every shop as a machine that does everything. It’s good to have friends in the industry.
If you have to flip it, you have to flip it. It’s square all six sides and be all careful about it. You can also use the dial indicator to verify it’s square.
The end mills deflect, so you’ll want symmetric depth cutting.
I know this feels like a frustrating limitation that should be easy to overcome but repeatable and stiff fixturing and alignment is probably the most difficult part of the craft.
