I’m interested in this topic as I will be shooting for 0.001" (0.025mm) tolerance if I can get it.
I like using the gage block as the “feeler” rather than paper that is 0.004" thick.
What I was referring to in my post was this. Hopefully it will help someone.
In the top image I’m shooting for a 4" block with a 2" hole or slot machined from both sides.
If my zero is not nearly perfect, I exaggerated and used a deviation of 0.1", the misalignment will be double the error.
In the second image, if the workpiece is off, you also introduce some error.
And in the 3rd, if both conditions exist in the same direction, you are now compounding the error.
@Tod1d I’ve spent lots of time thinking about whether my approach doubles errors, and every time I try, my brain melts and I am no longer sure.
I think XY errors are not doubled, because it doesn’t matter where you machine your reference corner in the first setup. You can be off by an inch and it won’t matter, because in the second setup you are placing the machined corner against the XY zero. What I think matters is that you get three flat surfaces and that your model is positioned correctly against these surfaces.
I think the same thing applies to Z: if, in the first step, you cut in too deep, it won’t matter much, because you will have cut in too deep on both the model and the top surface. After the flip, you will get the error, but only applied once, not compounded.
But as I said, my brain melts when thinking about this.
Jan, I drew that out for my own benefit as well as anyone else’s
I’m sure I’ll be experiencing the same brain-fry when I get my machine next month.
The doubling error would occur when XY zero is not perfectly aligned with with your guides.
You eliminate the 2nd condition by machining your J corner for the next setup.
But if you’re not putting that corner at exactly X0Y0 when you flip it…
I like that you mention also machining the top surface & not just assuming it’s perfectly flat & level.
Have you used a good square to check that the outer walls of the part are fully square with the faces which sit on the spoilboard? (also, did you surface the spoilboard recently? Is the machine trammed etc. ?)
I’ve done a few of these setups with Aluminium and what I found worked well for me was to
Add an additional MDF to the top of the spoilboard, surface it flat
Bore it for locating pins (in the Y axis not X which is unreliably square with Y)
Machine the front and left edges of the fixture to set zero from, also to align with a dial gauge if I need to remove and replace the fixture (again, test in Y only). I add some superglue to the ‘square’ corner and to the dowel pin holes to reinforce them before the finishing pass, make sure you let it dry properly.
Bore the part, only needs to be approximate here
Locate the part on the pins, zero off the left and front edges of the fixture (using an edge finder in my spindle, not the bitzero and a dodgy sized cutter whose flute angle influences measurement)
Machine the part, flip about the pins, re-zero from fixture if you’ve power cycled or pressed STOP on a job and had the Shapeoko re-zero and introduce errors that way
Ugh. I think my computer might have lost power between finishing that, making it, posting this, and now. I also see nothing in my manufacturing tab, not even a setup! Shoooot. Let me fix that tonight and get back to you.
With my revised process, I’ve been doing the contour from the top as well, which lets me study for overhangs in x and y, and from there I can shift the zero points slightly, re-run the contour, and wait until both sides are flush. I’ve been finding I need adjustments between 0.05-0.25mm range.
Since it is not consistent between my attempts, I lean toward @kelaa 's assessment that I’m probably just struggling with positioning/clamping repeatably after the flip. It’s somewhat close in x and y, but not always identical between the two (sometimes I adjust y by 0.05mm, x by 0.15mm to get my contoured profile from side 2 to yield flush sides).
If it’s really a 0.25 inch of error…
It’s 0.25mm And not even always; sometimes more like 0.1. That’s what this was meant to show (that hairline along the curved edge just below the halfway point):
I’m inclined to agree on compounding, and tried to convince myself that here when I was chasing the possibility that issues were coming from my axes not being perpendicular. Take a look at my attempted illustration here.
I still feel some brain hurt about the angular case… but I agree they aren’t doubled in this case. The part should be at (0, 0), but with this technique, the first side is irrelevant since wherever it is, the locating geometry is machined into it. Upon flipping, if either the machine or the part aren’t really at (0, 0), that’s the error, but that’s all the error there is. Either the machine needs to be aligned to the true (0, 0) of the part, of the part needs to be moved to the current true (0, 0) of the machine.
At 0.25mm, I agree that it’s probably repeatability of the second side setup. Endstop repeatability could also be an issue. If your machine homes between jobs and the end stops are randomly off by +/- 0.25mm then it would be a problem but more likely is just the physical process of trying to place it down and secure it for the second side at < 0.1mm accuracy. That’s hard!
@crpalmer Ok, no promises this is exactly what I did the first time… but quickly updated this with reasonable toolpaths to show what I was doing. The link should be updated, I think? Otherwise, attached. Hope that helps and sorry about that. flip_test_piece v2.f3d.zip (282.8 KB)
One thing that stands out when looking at it is that you’re using the model height == stock height. If that’s right, then you first surfacing operation isn’t necessarily removing anything. I’d try to leave a decent margin of extra stock that you remove. If not, then the stock needs to be exactly parallel to the build plate or else there will be a slight angle on the sides.
I’d personally like to leave at least 0.5mm to ensure it gets level and I’d happily leave more if I can.
That said, I still think that the placement and securing of the part after flipping it is the most likely problem. When I first tried to flip (using a SMW vice), I found I couldn’t do it accurately because the jaws would clamp into the part in some random amount. So, even though my y zero was “known”, reality didn’t match what I thought I knew because of the clamping pressure.
Similar idea, where the side 1 position on the wasteboard isn’t critical as you are machining the side 2 locating features in on the spot. That said, the dream process is:
pick a location for the left locating pin hole, set as xy=0
machine locating pin holes in waste board
tape+glue hold down piece so the side 1 origin is CloseEnough over the left hole
pull the piece, insert locating pins, and push the just-machined holes onto the pins
My issue was simply that I couldn’t get the pin fit right. Maybe it’s my OG z-axis flexing and yielding tapered holes? I could either pound them in and then really struggle to get them out, or have what felt like the perfect snug fit… only finding out after some issues that I could definitely still “wiggle” the piece a bit, meaning I was introducing the possibility of angular offsets.
The bottoms of the pieces nearest the origin would look great, but the pieces further away, as well as most/all of the heads would have a stair step. Folks are saying 0.25mm is pretty good… but I’d then chuck these on my drill press to sand, and found it took quite a bit to get a 0.25mm stair step out of a piece like this.
I’m definitely shooting for better. Give this a whirl and see what you think! So far I see no reason that dowels are any better, unless I got e.g. one of these aluminum wasteboards with perfect holes, or could bore perfect holes. I had to bandsaw some of my pieces right up to the pin to get it out. No fun.
Yeah, sorry about that and it’s deceiving. I do that just to simplify the stock setup. When I first put a new piece in there for side 1 machining, I touch off on the surface and then set z to e.g. 0.25 or 0.5mm. From there, the contour and adaptive are at the model height, and I touch off on the exposed “support” for subsequent operations (using other bits in real life on my chess knight).
Good observation about the clamping. I’ll have to study that more… I really like @jwr 's setup with the metal square and either the full aluminum wasteboard or that insert or what have you. I had really good luck with pins for the first chess set I made, so honestly I thought this much offset was me not catching e.g. some modeling error (not actually modeled symmetric) or a mental error going on with respect to flipping? I still think I should be able to do better than 0.01in… but now that I realize I’m getting close to 0.005in, I guess I should be happier!
@jwr Ok, making a knight right now with your “gauge block” idea… and I love it. I have a 5mm dowel pin and it indeed works awesome to just and roll it back and forth under the bit as I drop by 0.025mm. When it just touches, I just set z=5.01 (what I measured) and go!
I could already tell that I wasn’t being consistent between my main detail pass with a 0.125in ball end and the final details put in with a 0.5mm tapered ball end mill. I’d been struggling with the final pass being just a hair too deep, which is annoying to sand out. I just used the dowel trick for the first time and it’s perfect.
After somebody else pointed it out I bought a 5mm reamer to open the locating pin holes out to proper dimension, I bore them with the CNC and then finish them manually. A reamer gives you a hole which is the same diameter all the way down.
That sounds to me like the X rail might not be square with the Y rails, I’ve had that problem and now manually check the squareness on startup for jobs where it’s critical. The problem on a Shapeoko is they don’t always start up with the X at the same angle.
I’ve done a bit of flip work and find that setting my origin to be inline with the center line of the 2 pins helps me get a step free result.
Cheers Mike
Cool idea on the reamer. I’m familiar with them, but hadn’t thought of using them to take a hole to final diameter for this purpose. Neat idea!
Indeed, I think I did have an x/y perpendicularity issue, which I [mostly] fixed with some shimming. Looks like we engaged on that thread too That said, the evidence there was a stair step that changed along the y direction of the piece. The step on my pieces now is consistent along the piece, so I think it’s just about xy repeatability/locating, not angular deviation.
Question for you. I’ve been using the steel dowel trick for zeroing z but run into tough calls for in between land. What do you do in this situation? I’ve had positions for example where bumping up 0.025mm doesn’t cause contact but lowering it won’t roll under the bit. I’ve had others where I can just feel it contact as I roll, and middle ground where if I put a bit of downward pressure on it, the bit will roll under pretty nicely.
Is your process that sensitive, or do you just use this as a go/no-go? I can tell that being off by, I’d guess, 0.02mm for my final detail pass with a tapered 0.5mm ball end bit looks much worse if I end up too low after the previous 0.125in ball end operation.
My best guess has been to start trying to learn half steps… like if I step in -z and it’s a hard stop, but +z one step completely clears, I might go +z so there’s no contact and call that z=5.025 (my true dia is 5.01). If it just kisses the pin with no down pressure, 5.01.
Thanks for any tips if you’ve run into this. If the machine can only step in 0.025mm steps, it made me wonder if this is why your bit setter was unreliable? I don’t have one, so not clear to me how it determines z=0 with respect to the machines step size limitations.
I found that I’m getting good results by being consistent and following this rule: always start in a position where the gauge block doesn’t fit (e.g. lower XYZ value) and increase X, Y or Z until I can fit the block “reasonably easily”. There is usually a position where I can force the block in, and another step or two up where it goes in with a bit of friction, but easily. That’s where I mark my zero.
I never go back a step, this makes no sense, as the backlash will eat the results alive If I have to restart, I go back a significant amount, change direction, and then repeat the procedure.
I should probably try going one more step up and see if I get a difference in stepping on the finished model.
I don’t think I can get much better given the build rigidity of the Nomad. On a Shapeoko I think things will be much less precise.
Thanks for clarifying. Ah, that’s very interesting and I hadn’t considered backlash! By this:
I never go back a step, this makes no sense, as the backlash will eat the results alive
You mean you always go to a “no-go” stage, then creep up until the block goes? (Just calibrating what you mean by “back” vs. “forward”)!
I don’t think I can get much better given the build rigidity of the Nomad. On a Shapeoko I think things will be much less precise.
Hmm, good point. I forget you’re on a Nomad. By using my not-systematic-at-all method below, I’ve been pretty darn happy on my SO3 XL:
drop down in 1mm until the pin doesn’t fit
go up by 0.25mm until it easily fits
drop down by 0.025mm until I just feel the bit rub
That’s the ideal anyway. What I find is that I can go down, feel nothing, then go another step and it feels like too much friction. Because it’s been surprising to me how drastic one 0.025mm step can be, I’ve even gone back and forth and verified that, indeed, I feel nothing at one position, then too much resistance for my taste at the next lowest.
I’ve then usually been going back up and calling that 5.02 (add 0.01 to the diameter), or if it’s just rubbing enough for my tastes, I’ll call that 5.0. If I can barely perceive the blip when I roll under it, I go 5.01 (exact dia I measured).
This is purely Z, though. I have been inferring x/y by contouring and chasing any overhangs by manually adjusting and re-running. Once I get a more sturdy square I can try your method on x/y as well. Still, the contour is the most direct answer to “am I where I should be” so I might not get away from it.
And not even always; sometimes more like 0.1. That’s what this was meant to show (that hairline along the curved edge just below the halfway point):
