EDIT: It turned out to be a loose lead nut. By loose, it wasn't firmly attached to the gantry. Hey guys, I hate to have to start a thread on this, but I need a quick answer. Is this backlash or a gcode error? I'm using Fusion 360. The entire cut is made with a ramp operation. The estimated time is ~7:30. If I keep the ramp and set multi-depth, the time jumps up to ~20:00. I did not try the second method as I don't have the time for that with the shear quantity to be made. Plus it shouldn't need to do that to be made correctly as the gcode preview shows the same line. The result can be seen in the first pic. The piece to the left was the first attempt. The piece to the right was the second attempt. The only difference was that I activated smoothing. The second picture is a previous cut using SketchUCam. The part itself doesn't have the same finish for a variety of reasons, but the main thing to notice is that it's actually a circle. The part is a 26mm diameter spacer with 4mm width pockets. It's being cut with a 3mm o-flute. The machine is a Sphinx made from 500mm extrusions. Up and down in the picture is the Y direction (double lead screw). Taking this thing apart just to get to the nut is a nightmare. The attached gcode is for the 4 cutouts and the outline. Any ideas? Edit: I'm asking because I can't physically find any backlash in the machine. Plus I rebuilt the X and Z axis very recently so there is zero possibility there.
Three things to try: (1) Make sure your Y-axis is square with respect to X-axis and that Y-axis rails are parallel to each other. (2) Make sure you have calibrated the steps/mm for both X and Y axes. And that you have measured them independently. Don't assume that they should be the same value. (3) The bit and your machine goes through the most stress when ramping. So making your entire cut a ramp seems like it might be causing deflection. Try cutting a circle (or square) with a lead-in and lead-out and ramping during he lead-in and lead-out. For this test, you only need to cut a single depth-of-pass. If the engraved square or circle is accurate then it is likely that your machine isn't rigid enough to handle the stress of constant ramping and is flexing under the load. Best of luck. -D
How are you checking for backlash? best way is probably with a dial indicator.. if your "anti-backlash" nuts are set too tight you will have a bunch more backlash than if they are too loose.
So after studying both of your replies for hours, and double checking and applying everything, the expected problem is simple. I don't quite understand how, but the lead nut on the X axis was loose. It wasn't firmly attached to the gantry plate. And notice that I mentioned recently rebuilding it. I didn't think to check that....again. I just tightened it back up and will give it a spin. I did go back to SketchUCam for a comparison. The results did not change, but looking at the two cuts overlayed was the ultimate "this is purely mechanical" indicator. (I cut the same part with a 45 degree twist on a previous cut.) I'll give it a spin and report back in a moment. Thank you.
(1) Good enough for government work! In all seriousness though, they are indeed aligned. I don't have really precise tools to confirm, but to the best of my abilities while testing the machine has reinforced the notion that it is indeed square. (I realize that's kind of a stupid answer.) (2) Make sure you have calibrated the steps/mm for both X and Y axes. And that you have measured them independently. Don't assume that they should be the same value. Calibration between all three axis were done independently. (3) Now this is where I have to disagree, but first I'll state that did eliminate the ramp as part of the testing. Ramping has been the best thing I have ever done with machining aluminum. You're actually reducing the harmful load from plunging. The effectiveness of a ramp highly depends on the tool. Some tooling is capable of angles as steep as 10 degrees, while others should be kept at a conservative 2 degrees. I run either 3 or 4 degrees on an o-flute, but they can handle more. The chips are smaller than normal due to the fact that back end of the cut is removing less material than a proper parallel pass. Although I said I disagree, it just depends on the application. Some tooling is an absolute no go, which is why we drill with a separate drill bit, then insert the end mill into the drill hole for milling. As for the flex, I normally run much much harder. Normal operation is a 1/4" at up to 10mm depth for a finishing pass, or 3mm for clearing. I'd break the baby 3mm mill long before the machine feels it. I really need to invest in some proper tools. During the double checking, I actually did set one side of the Y too tight and it actually seized on me. Fortunately, squaring the machine again is quick and simple. Here is the result. Yes it is off centered do to the drilling operation being wobbly, but I can compensate for that and do the four rows individually. (Ignore the extra drill hole. I set the model offset incorrectly in the beginning.) Again, thank you guys! Kevon
looks much better, what O-flute bits are you using (where from) and the actual numbers of your DOC, rpm, and feed and speed. thanks
For smaller parts: 3mm OD O-Flute (exact end mill) At full width: 20k RPM 0.7mm DOC 550mm/min Feed 500mm/min Ramp 30mm/min Plunge Flood HSM Method 20k RPM 2mm DOC 0.5mm Stepover 500mm/min Feed 500mm/min Ramp 250mm/min Plunge Flood I get some nasty power fluctuations so I keep the speed higher to account for the drops. Sadly, I'm still using a Bosche Colt. The poor thing is almost dead, but it hasn't bought itself a replacement yet. It can run harder than that, but then simple variables begin to make huge impacts. Tooling is not made equally! This particular supplier for this particular end mill has been golden. I get all three sizes for that link. I also get diamond cut (corn) end mills from them. The smaller sub 1mm end mills are hit or miss. My larger tooling comes from LakeShoreCarbide or 2Linc. The finish isn't near polished like the larger 1/4" finisher, but that's a multi tool process. O-flute are more for material removal, not finishing. As for those specs, I won't post due to safety reasons. The little 1/8" and below stuff will break, but a wrong move with the bigger end mills will break the wrong side of the operation, so it's better to take a more personalized learning approach with them. The part on the left was made will dull tooling. The right was made today. It has some use on it, but not nearly as much as the left end mill. You do see horizontal lines. That's not normal.
Nice! thanks for the detail, I've been looking for an o-flute that's not super $$ and those look like the best price I've seen. I just wish they only had about 3/8 of doc instead of 5/8" but if they work...Nevermind I see the description is different than the actual, the DOC on the 3mm is 0.47"! I also see they have Ti coated 1/8 o-flute.. Great source! I just ordered 6 of the Ti-coated 1/8" I have never had luck with slotting in aluminum (belted OX), Maybe with a good O-flute I will, i know they work great on acrylic. I've had luck with Estlcam, makes trochroidal milling so easy I was able to do 1/2" aluminum with an 1/8" bit and no chip welding. Also I don't have the ability to flood cool like you do. Are those motor mounts for RC planes?
Perhaps I misunderstood. It sounded like you were constantly ramping when cutting out these parts, essentially cutting in a large spiral. I'm used to doing a ramp (never a plunge) and then cutting at a constant Z for a layer. Then ramping again. And on harder materials, I would consider doing the ramp on a lead-in (not on the edge of the part) so if there is an issue during the ramp it only messes up the scrap and things are at a constant Z for the whole outline of the part. Since we now know that ramping (or not) had no impact on your problem because the root cause lay elsewhere, I'd like to know how your successful cutting went. Was it ramp-flat for a bunch of layers? Was it spiral-always-ramping? -D
DO NOT GET THE TI COATED MILL!!!!! Remember all tooling is not made the same. The same can be said for coatings. I tried them and they were utter garbage. Stick with the plain uncoated mills I linked. I used the one sI ordered as Dremel bits since I can't use them for milling. Aluminum and plastics do have a surprising amount in common.
You understood correct the first time. Because of the shallow ramp angle, the side engagement could be set to a constant depth. For this particular piece, I unfortunately couldn't apply a lead in, but I do agree that having a lead in saves a lot of grief sometimes. The part finish is also better at entry. As for the final result, it was done with a costant ramp as well. I don't mind dropping to a height and passing, but the time it requires just can't justify it. This is a hidden part so it's purely there for a function.
I did, not a big deal if he already packed it, I do more plastic anyway, I’m sure they will work fine for that. Thanks
Jason at Drillbitsunlimited.com got back to me fast, I was able to change my order and I ordered some 2mm and 3mm of the O-flutes. Great service! I will be using them more. Thanks for the tip Kevon.
titanium nitride coating (the yellow one) do not work well with aluminum. some chemical reaction I gather.
You might be right, found an interesting chart on coatings.. Harvey Tool - Coating Chart for Ferrous and Non-Ferrous Materials
You also want to avoid any aluminum based coats. Similar metals will literally transfer from the tool to the work piece. That means uncoated beats AlTiN and TiAlN when cutting aluminum. I use TiCN, ZrN, and Diamond. There are also two types of diamond coatings, but I can't remember the exact details off the top of my head. Another thing to consider is heat. Some coats actually need to be hot in order to function properly. Just look at videos where they are sparking through steel dry vs others that flood the heck out of the work piece. Titanium coatings TiN, TiCN, TiAlN, AlTiN - HANNIBAL CARBIDE TOOL, INC. I'm glad this thread became useful. . Now if only I could change the title...
