Okay, this is a weird one I guess. I tried to cut a blast gate, pretty deep (18mm) with a 3.175 endmill. The measurements of all the parts are nearly spot on but the fingerjoints, which are off.
Let me explain: The gap in this picture should be 2.635, it is 2.56ish.
This is the part that has been cut out of the above gap and it is 1.935ish, should be 2. So the endmill took out roughly 6.35mm. The error therefore is consistent without runout.
Now you are gonna say: Well, your measurements are off, the MPCNC does not cut 10cm if it should have cut 10cm. But no, it isnât, all the other parts are correct.
Now letâs look at the cutout for a fingerjoint. Itâs 2.1cm, should have been 2cm. So it is off in either direction, fingerjoints are too small, fingerjoints cutouts are too big.
I thought maybe the problem is with the âFreifrĂ€sen (Overcut in English)â, that it does the overcut but does not really go back. At least it looks like it and I donât know why. That would at least explain the consistency of it being off in either direction. Any thoughts would be appreciated.
/edit: Looking at my French Cleat, the problem seems to be worse the thicker and maybe harder the material is. Kind of weird. Did anybody try it with a finishing pass?
One of the common issues Iâve seen is âholes too small, parts too bigâ which is the opposite of what youâre seeing, but I think could be related.
The CAM makes allowances for the bit size. If you have more runout in your spindle/router than expected, the actual cutting diameter is going to be larger than your CAM has allocated for.
Or maybe the bit is just larger than you have set up in your CAM.
I suggest that you try to just cut a groove in your material, and then measure the actual cut width. I commonly get a measurement of almost exactly 3mm from my 1/8" (3.175mm) nominal cutting bits, and I get good fit for parts when I tell the CAM that itâs a 3mm diameter bit.
It looks to me like your bit diameter is understated, and your cutting width is greater than the CAM is accounting for.
I am reading through your description and getting confused. So please be patient with me if I make a suggestion that doesnât apply to your situation.
At one point you saidâŠ
Did you mean it took out roughly 6.35 mm by error? Because that is a LOT. That is double the width of your bit. That would be caused by CAM telling the machine to use the bit on the inside of the line instead of the outside of the line.
Nah, it takes 3.175 on each side, doubled that itâs 6.35. Sorry, I was not very clear. First thing I did was to check whether I accidentally set it on the line and not next to it, but that is right also. So there is no runout at all.
But maybe Dan is right and it is smaller than it should be, though thatâd really confuse me a lot. Going to measure that tomorrow. This is what makes most sense, though it really looks allright, since 3.175 is pretty straight.
Updates tomorrow. Thanks for your input!
I still think it has got to do sth with the Overcut (or dog bones, how do you call it?). You can see, especially in the third picture, that there are the corners that are cut out further, then it goes back in and then immediately out again, even further than the cutout of the corner. This should not happen. It shoud look like those:
You have to zoom and squint a bit, but you can see that all the edges are straight and the corner is cut a little deeper. This is not the case for the cuts above.
I see what you mean. But that looks like âFlexâ in the machine to me. If the bit is always deflecting in some direction (usually lagging behind the current move) but the machine slows to a stop at a corner then the bit will have a brief moment to straighten before the machine can accelerate in a new direction. That will give you this kind of affect. And the direction of the bit spinning will also make it flex to one side as it starts to move again. I think Climb vs Conventional milling can affect this more or less but I could be wrong. I think the most common solution to this is to compensate for the flex in your machine by changing the size of your bit in CAM as well. Unless there is a way of using a finishing pass for Engraving that I donât know about. I see the option in ESTLCAM but I have never noticed that it had any effect on an engraving cut.
Itâs not an engraving cut, I already programmed two new parts with 0.5mm finishing pass. Also going to try that tomorrow.
What you say could not really be the fault, can it? The depth of the pockets is exactly 10mm as it should be. If it was flex it would not. But I will keep that in mind and also check that. Thanks!
That is exactly what the âovercutâ is for, to remove material that would have been left because the bit is round. Estlcam should show you that in the Gcode preview as well. A small deviation in the corner where the tool moves slightly outwards into the corner in order to finish clearing away all of the material inside. This is very useful for things like finger joints, because you donât want the slightly rounded corners interfering with assembly. The overcut will remove a bit extra material to make sure that the part inside the finger joint is entirely clear. The alternative is to either file or saw out all of the corners to get a sharp corner, which the round tool is inherently incapable of doing, or else to file or sand down the fitted corner to the same round profile as the tool leaves. Both can be a lot of work, and difficult to be precise. Cutting into the corner a little bit automates this.
I use this feature in Estlcam quite a bit for fitted joints, like the finger joints in my Repeat printer. It should not affect dimensional accuracy outside of the overcut area.
Thats a macro shot of the inside of my repeat printer where one of those overcut corners is. I know itâs there but most people will never see it unless itâs pointed out. But theyâd sure see it if I didnât clear those corners out.
I think a finish pass on an engraving cut is slightly deeper, not offset like the finish pass on a part or hole cut.
Anything that needs to be dimensionally accurate should get a finish pass though.
Thanks, I know that. I somehow sound more dumb than I am I guess⊠In the additional pictures I posted it does exactly that. It takes a small circle out of the corner and then goes back to the original path.
With the wrong parts above, it does cut out the small circle but does not go fully back to the original line but stays at the level of the cutout.
Here it is right, cutting out the corner and going back:
Here it is cutting out the corner, but not going back, it is staying on the âlevelâ of the cutout. Green in how it should look, red is how it does look, basically straight.
I have frequently been surprised by things that I thought I knew, but were different from what I expected. I had no intention to offend.
This is sounding like something not tight somewhere. A little slack in the belts will give backlash problems, which can display differently for conventional or climb milling. Similarly bearings which are not tight to the rails allow the core to move in differnt ways and will present themselves as other kinds of problems. Something isnât moving as commanded.
Iâs unlikely to be the motors or control boards. Those tend to be large problems. Iâd also discount the possibility ofthe ever popular grub screw as the problem, as these are maddeningly inconsistent. To me, this looks like a backlash/flex thing.
Belts. Slack in the belts will present as this sort of issue, where cut dimensions are off, and right hand corners will present differently than left hand corners, so in a finger joint, the ones sticking out (left, right, right, left) will be off differently than indented (right, left, left, right) â this can be reversed for climb milling and conventional milling. That might be a reasonable test, to reverse directions and see if it follows. Overcuts kind of gum up the works, because the tool reverses direction momentarily.
Next is loose bearing contact. Check that nothing goes âclunkâ or rattles when mild pressure is applied to the tool head with your fingers (Obviously when the tool is off!) Make sure that all of the core bearings and truck bearings are in contact with the rails. None of them should be able to roll easily with a finger without actually moving the machine.
And finally, check for build tensions. I know that Ryan has often said that nothing should be anchored to the top of the Z tower. Even a drag chain can have a fair amount of pull on the axis at the end of that nice long lever. Make sure that all of the rest of the machineâs action is free and easy when unpowered.
I know, I am sorry I might have sounded too harsh, wasnât intended to, I really appreciate the input.
I measured a cut today and it was roughly 2.95mm, so quite a bit off. I will adjust for that next time and see whether that works. Or just order a new endmill.
You can also view the gcode in a visualizer like ncviewer to double check whether its doing overcuts. It sounds to me like deflection, and a finishing pass should clean it up.
Do we have a video how the belts should âreactâ or âbounceâ. I think mine are okay, but all my screws were too loose when I started 1.5 years ago, because I was really gentle.
Aaaaaaaaand, ladies and gentlemen, we have a winner. It is @SupraGuy with his well-informed answer that the belts might be too loose. Never would have guessed that, because it is only really noticeable for those cuty, nowhere else.
I will adjust for that next time and see whether that works. Or just order a new endmill. 
