Hey all, I have an Openbuilds Lead 1010 machine and am using Fusion 360 for this - I’m working on a guitar neck/body and need to be able to flip the piece and have it cut exactly the same on the other side. I’ve done everything I can think of and can’t get it to line up 100% or even 99%. I get about .005 difference every time and not sure how else to proceed. I did a test piece today using a different alignment method. Instead of ¼ holes/pins straight up and down from each other, I did offset holes like this: On the necks, I was going dead center above and below in the stock so that when I flipped the piece, it should line up perfectly when flipped. But every time, it’s still just slightly off. I know there can be a lot of variables, but I’ve calibrated the machine, made sure it’s square and all I can think of. So to test, I just did this rectangular piece to see if it would line up -- it does the same with the .005 difference. Almost exactly the same on both Y-axis. X-axis seems good at the very bottom -- but not at the top of the piece. The cut seems perfectly straight so that’s all good, just slight off. And I’m not leaving any stock to leave in the job either. Just a basic contour on each side just over half way so I can see where it meets up and what the difference is. I’m also zeroing off of the “fixture” the same way every time. This is what it looks like when I pull it over afterwards. See how the top cut and bottom are off from each other? Any help would be greatly appreciated! Thanks again! I have the Fusion file as well if you need to check it and see if I'm doing something wrong.
What are you calling the fixture? Are you zeroing X & Y, or just Z? Chance are that there is a (small) discrepancy in the position of your locating dowels between CAM and reality. ETA: Feel free to post the F360 file and I'll take a look.
You can see the zero in the first pic on the fixture. when I do the other side, I'm flipping the fixture, but keeping the same X and Y since the fixture is perfectly centered as far as the dowels go. I also had the CNC re-bore the holes before started just to make sure that they are lining up to the same spot. I know I can probably just contour all the way through and resolve the issue, but wanted to make sure things were centered since as you know on a guitar neck of all things, the carve on the back really needs to be centered. I'm attaching the Fusion file to help -- I pulled most of the guitar related stuff out of the file, and left this test piece that I was doing a similar thing on -- but I did move the alignment pins to offset each other to try a different approach. I can also add the original one as well if need be.
That will only work if your fixture is also *exactly* 7.000 inches wide in real life - any error between what you tell F360 that it measures and what it really is will get doubled when you flip it over. I've looked at your F360 file, and while it it is a little bit 'busy*' ( ) it looks like it should do what you want, but is critically dependent on the actual dimensions of the fixture matching the CAD/CAM dimensions (since the edge of the fixture determines the origin). I'd suggest putting the locating dowels on the centre line and using one of them as the CAM origin - that way, the fixture dimensions get taken out of the equation. (*I notice a lot of 'moves' in your design - strongly recommend learning about & using 'joints' to position things accurately and reliably - 'moves' have a habit of coming back to bite you eventually! )
Ok thanks for the info -- yea, this file is actually much larger since it's a whole guitar and all the parts for it. I did cut the fixture from Fusion on the 1010 so it should be tight, but when I flip the piece I'm not actually re-zeroing the X and Y, just the Z since theoretically it's the exact same size both ways. And I would assume that would take that factor out of being not exact. So I would assume since Fusion thinks it's exactly 7 inches and the flip is theoretical, it would be good? So when you say center the dowels and use one of them as the origin, you mean setting the X and Y to that dowel center? As far as moves, I assume you mean the fixture? Yea, I'll have to read up about joints. Most of this is definitely all new to me, so I'm still learning for sure. Just ran the test again after re-homing in between flips and the X- axis part looks pretty decent but the Y-axis runs are still off by the .05 or so. Weird.
That's the way to do it. Good in theory, but not necessarily in practice - F360 is putting the centre of the part at 3.5" from the origin (being the centre of your theoretical 7" fixture). If your zero point on the machine isn't exactly 3.5" from the dowels (if the fixture isn't exactly 7"), you'll get a mismatch when you flip. Yep. I didn't drill down to see what they were, but in general, they are a bad idea. Model each part, then align them with joints. You're flipping the part about one axis. If there's any centring error it will show in the other axis.
Ok - so in fusion, when I do side 2 (the flipped part) I should re-zero off of the center of the bottom dowel hole? Or should I do that on both sides? In other words, if I used 2 dowels, top and bottom of the extra stock above and below the actual piece that's being cut out - centered, I should find the dead center of those and set the zero x and y to that part? Like this?
But if I don't change anything about the zero - and it bores the hole at the 3.5" mark, then when I flip it, if I don't touch the zero, it should be exactly the same since the zero wasn't ever altered and the piece should contour exactly perfectly along the Y-axis unless it's something with the machine possibly?
You're setting your zero off the fixture at the moment, aren't you? Exaggerating: Suppose your fixture is actually 6" wide, rather than the 7" that the CAM is working to. You set your workspace origin on one edge of the fixture. The holes will get bored at 3.5" from that edge, which is 0.5" off the centre line of the fixture. When you flip the fixture and locate it on those same holes, the part will be 0.5" on the opposite side of centre, leading to a 1" mismatch between the first side and second side operations.
On two-sided parts, if the alignment holes are drawn as part of the model then copied to the other side, you are correct in that you do not re zero x and y. You cut side A, remove the part, load side B file, drill holes that were copied from side A into your spoilboard, insert alignment pins, flip and align part, re-zero Z then cut side B. I use at least 3 pins when I do this process. Broken endmills work great. Especially if they are the same diameter as the endmill you are drilling the alignment holes with. I believe what we are both describing is essentially this process where no fixture is needed. That eliminates any alignment error or measurement errors on the fixture.
Thanks again for all the info - yea on this piece at the top of the post, that's exactly what I did. Didn't use the fixture at all - drew the holes into the piece of stock that I used as the "stock". Drilled the holes half way thru the top side, cut the contour about half way thru, took the piece off, never re-zeroed anything. Drilled the holes into the spoil board directly, flipped the piece and put it in the holes on the spoil board, ran the back side contour and was off the above. So it would seem the process is ok?
That wasn't the setup in the F360 file that you posted. Again, if you're setting your machine zero using the edge of the stock for this sort of operation, the stock needs to be *exactly* the same size as what you have assumed it is in CAM. If not, you will get double the error as a mismatch when you flip it.
Is your machine accurately calibrated? If it is off and cuts slightly too big, then it will be off by that much just like you showed if zeroing on a corner. If you zero in the center, it should not be off. And that center can be anywhere you say as long as the stock is big enough. Check calibration, or do the same process, but flip end for end rather than side to side, or zero in the center.
Yes I did check the calibration and it's pretty good - pretty much dead on. I did check it over a 600mm span. Yea I guess I could try centering it based on the piece - guess it only needs to be centered on the x-axis plane since it's going to be flipped?
I usually make the job origin the center of my material (X and Y). It does not have to be precise as long as you have enough allowance on all 4 sides. After that, the alignment holes should take care of everything else. I zero on the machine bed for Z because that way I do not need to worry about having uncut material for zeroing Z if some thing catastrophic happens and I have to recover a job. Think about scaling. If your calibration is off by 10 percent (Just a simple number I made up) and you start in the center, all you did was increase the overall size by 10 percent. The error is equal all the way around. Both sides cuts should line up. If you only zero on the bottom middle (X but not Y) and you are off 10% on both axis, when you flip it you will be off on one of the axis by 20 % because you will double that error of that axis.
Right on -- I've always zeroed off the bottom left -- so going to try the center zeroing instead and see how things go. Probably going to stop using the fixture as well. I was doing that since I saw a YouTube guy explaining that he's using that since his stock is not always flat and this way you'll be more accurate since your stock is not always planed and totally straight. Made sense, but I do feel like the fixture has definitely complicated things more. I'll just use the bed, like you were saying as my zero for Z and center it for X and Y. So I don't need to be totally exactly centered when I set the X-Y? I guess since I'll be using the same zero when I flip it probably won't matter? Also, I didn't necessarily need to change the zero when I flip the piece from the bottom of the bed to the top of the stock? Sorry - still pretty rookie-ish. Thanks again.
Ok - tried new zeroing based off of the center of front edge on both sides -- so basically here - then flipped and left the zero exactly the same only re-zeroed the Z axis since I did a bit change for the holes. Now it's a little closer but still off a little. The interesting part is as it gets closer to the back to the piece, it gets better. One small part of the back side is almost perfect. Here's the front Here's the back And here's down the side -- you can see as it gets farther back, it seems to get on-track What do you think would be causing that? I checked for the squareness of the table/CNC and it's pretty close to dead-on. This top side is also the second (flipped) cut. I'm thinking about trying from center of the stock now to see if there is any difference. And I didn't go dead-center of the stock for the zero plane since I didn't touch it in-between cuts, so figured it didn't need to be dead-center? Thanks as always for any insights! Getting closer.
you absolutely must set XY zero and THEN drill the pin hole at that position, and after that mount the material and then drill the pin hole in the material (seperate Gcode jobs) so that when you turn it over XY has not and will not change. If you do have to reset XY (because of a crash, then I would move XY a little and drill a new holes and put the material on that new pin. I have done it this way, and I have done it the 'fiddle around trying to find that exact XY again' way, and just redrilling the pin holes is much better and faster.
Right - this is what I did - set the XY - drilled the holes in the stock and top contour about half the way thru the stock, took it off, drilled the holes into the spoil board, flipped stock and mounted, and ran backside contour job a little over half way thru the material and this is what it came up with -- getting closer but wasn't sure if I should try zeroing off of the center of the board instead of just zeroing off of the edge like I did?
it is critical to do several things that act in concert: in CAD, place 2 pins on the centerline of the object, in the same place on front and back, so that you see the same pins from front and back place the 0,0,0 point on one of those pins, again on front and back using the same pin. generate Gcode to drillt he 2 pin holes in the spoilboard jog to the right place for the reference pin and setZero XY there, then probe the surface of the spoilboard for Z run the hole drilling Gcode to make the iniital holes place the material over the holes in the correct place for front side carve. generate and run Gcode to drill the holes in the front side run Gcode for the front side carve remove material place pins turn material over and place on pins, fasten it down run back side carve the above assumes you are doing bit changes and probing the table appropriately and have set the carving to have Z=0 on the table.
That's pretty much my process other than the Zero at the center of the pin - I'll do a center of the bottom pin (the pin closest to the front of the CNC) and try it out. So basically like this?
Exactly, yes. The pin is your reference point for flipping the stock, so use it as the reference point throughout. Alex.
Ok - ran the job based off of the zero at the hole and it's definitely getting better -- it's weird though the right side is almost perfect, but the left side still has a very small lip on it -- what do you think that could be? Also, both X-axis parts look pretty close as well. Just the left y-axis part. Thanks again!
probably bumping up on backlash now, and the direction of cut will affect the exact finished size. do a roughing cut on that outside edge, then a finishing pass CLIMB cutting on the front side and CONVENTIONAL on the back side might narrow that margin
Got another quick question for the group, why does Fusion show machine times much quicker than the OpenBuilds software shows once I start the job? Like for example, adaptive clearing in Fusion shows 16 minutes, once I load it in OpenBuilds software, it shows 33 minutes. Same speeds and feeds? Have always thought that was weird?
