I am still trying to get an inlay to work without success. I decided to go back and start simple.
Here is an egg shape that I pocketed and then parted another to fit together. Straight bit no carving. the image is 1 in x 1.5, I know its small. There is the slightest gap along the upper left side but npot much. I put no finish allowance in the cut. I expected it to be really tight but it’s close but not tight. My question is, is that within the +/- of the machine/bit or do I need to make an adjustment.
I would try to cut out a 100mm square or similar and see how close to ‘on dimension’ you are. If you cut it in both directions (one clockwise, one counter-clockwise) and they come out different, you know you’ve got deflection during cutting.
Having a finishing pass at ~10-20% cutter width helps a lot with that, assuming that it’s not deflecting more than that on the main pass.
Nice, looks pretty reasonable. Was that cut clockwise or counterclockwise? Also, was that using a finishing pass? For this test, a finishing pass would mess up the results.
The cut did include a finishing pass. Linear cut in X axis and the linear cut in the Y. I managed to get the homing on X axis to work so I repeated the process here are last results.
Uhh, is this a pocket or cutting out a square? I may not have explained this clearly enough, sorry.
I would do it as cutting out a square that’s 100mm using whatever settings you used above to cut the ‘plug’ for your insert out, no finishing pass.
The goal is to end up with 2 squares of material cut in 2 different directions, one clockwise, one counter-clockwise. Changing direction means that any deflection due to the cutting forces will also change direction. If your cutter is deflecting 1mm off the path then it’ll result in a 98mm square in one way and a 102mm square in the other. You’d then know that your deflection is 1mm, so you know how much of a finishing pass you need at those settings to fully clean it up to dimension.
From there it’s a balancing act… Cutting faster and leaving more room for a finishing pass is likely the fastest option, but having a finishing pass be a couple of mm is pretty close to your original cutting pass, which means it will be less accurate. Cutting slower and only needing to clean up 0.1mm is probably overly cautious, so you could get away with running the main cut faster and leaving a little more for clean-up, etc.
If your machine is not 100% dead square, some skew will also be present.
My machine is pretty good, but I still try to account for that skew by flipping the jmage for inner and outer parts, then rotate 90° to make the skew go the same way on both parts. I haven’t done this for inlays, but have for making boxes with shaped lids.
Now that is definitely an interesting result… Perhaps try stick a pen on the machine and see what it traces for a 100mm x 100mm square?
Ideally, you should see the machine trace a 100x100 square with the diagonals the same, then cut something like a 101mm x 101mm square using climb milling and a 99mm x 99mm square using conventional milling, which would indicate that you’ve got ~1mm of tool deflection under load.
Having it be different in the 2 axes isn’t surprising, now that I think about it. I’m a little more used to the MPCNC which is symmetric but the LR4 isn’t, so presumably that stiffness is when it’s trying to rotate the core around the Y axis, rather than pull the core away from the rail by rotating around the X axis.
The diagonals being different is a little confusing, although that could just be an effect of the deflection being more in one way than the other.
So looking at that, I’d assume it’s maybe drawing a 99mm x 100mm square with the diagonals off by about 0.5mm as normal. Either way, I think that looks like it should be solvable by doing either a 1mm finishing pass or 2x 0.5mm finishing passes.
You could also try slowing down the cutting a little and seeing if that leaves you with less finishing to do, which may be faster overall.
That’s a great sign. That means everything is working correctly in terms of the motion itself.
It may be that you’re just running a cut that’s a little too aggressive for your build/material/tools and either need to allow for a finishing pass or to take a shallower DOC, maybe.
I’d add a 1mm finishing pass and see how that improves things. If they’re still not quite on-dimension, I’d slow the feed rate down, try a new sharp tool or take a shallower depth of cut until it lines up with what I want.
Also, make sure the chips are getting sucked/blown out of the cut effectively, especially for deep slotting operations…
