I noticed last night that when I spin the collet nut by hand on my C3D router that there is a slight variation in the bit position. I put the deep sweep shell up against the bit and as I rotated it pushed that shell over slightly but noticeably.
There is no play in the bearing, nothing wiggles.
My machine is (or was) trammed really well and I have not noticed any of the telltale variation in surfaces.
I noticed this issue with both #201 and a simple steel pin. I plan to try a different collet and also compare to an older C3D router that I has the Makita rebuild kit in it.
What is the best way to determine the source of the problem? Is it possible that its a collet or that the bearing is slightly misaligned? I have not noticed this before and I did some inlays a few months ago that I would think would have been ill fitting if this issue existed then.
If you take the collet nut off, is there a concentric surface above the threads you could indicate to determine if the shaft is out? Or maybe an indicator on the inside tapered face / collet seat??
I will see if I can get my dial indicator arranged in a useful position. I don’t think it is the shaft but will check, The difference seems more pronounced at the bottom of the bit than the top. More like the bit is angled.
Problem solved, it is the collet.
Looking at the measurement near the bottom of the bit I got this:
compared to this:
The difference was slightly less at the top:
compared to:
I tried comparing the shaft which is a little tough due to the indents but it looked good. I switched to a different collet and got a difference of only .013 if I interpret the lines on the gauge correctly. It was basically just over one line different vs 14 which I think it .14
What SHOULD I expect? I know that my gauge being stuck to the 123 block with double sided tape is also a source of possible error.
Your last reading looks like 0.0095" ?? Tape isn’t going to flex that much, as long as the 123 block isn’t moving. Can you angel the indicator so it’s touching the tapered inside of the shaft?
Just as a sanity check!
If 2 collets are giving different readings, sounds like it’s definitely the collet.
Close inspection of collet & inside of spindle to make sure it’s not flaws, scratches, debris…
Usual preface, I’m with PreciseBits so while I try to only post general information take everything I say with the understanding that I have a bias.
This is a combination of angular/skew and radial/parallel runout. On that old collet you had ~0.009" of radial runout (if that was the measurement at the face) and were adding ~0.005" per amount of stickout from your first to second measurement. In other words you couldn’t get less than the 0.009" and would continue to build more and more runout the further away from the collet face you get.
As to the how much should you have (can tolerate), it depends on your cuts. Runout adds and subtracts from chipload (in multi-flute tools). At least until your runout gets to chipload x (flutes -1). After that you have a huge chipload (feed) on plunge and your entire chipload moves to a single flute. This all changes some back and forth depending on helix (flute twist), pass depth, and the position of the flutes relative to the collet and router bore.
To give a more practical example. Let’s use only 0.002" (0.051mm) runout and say we are cutting at 10KRPM, with a 2 flute and a 0.004" (0.102mm) chipload. That would work out to to 80IPM (2032mm/m) feed. In the worst case what will happen with this cut is that one flute will cut a 0.006" (0.152mm) chipload and the other will cut 0.002" (0.051mm). This is because as the tool is rotating it’s moving in and out of the feed direction. That means that functionally you are worst case cutting 120IPM (3048mm/m) on one flute and 40IPM (1016mm/m) with the other. That’s less than ideal for machine time, tool life, and finish. If the runout was 0.004" (0.102mm) or more then in the worse case you are functionally cutting 160IPM (4064mm/m) on one flute and nothing on the other.
What that all comes down to is that there’s a max amount of runout you can deal with depending on the cut. A decent way to set it up would be no more than X% of chipload depending on how much margin you have for minimum and maximum chipload (feed).
For the above I didn’t really touch much on plunge, some direction changes, chip form, or that you are also changing the cut material perpendicular to the cut direction. They are typically the more minor points and is more confusing than I already made this. But I wanted to mention that those are also issues.
Hope that’s useful. Let me know if there’s something I can help with or expand on.
I had a similar issue with my collet/spindle. I measured everything with a dial indicator and everything except the mill was dead on. I’m new to a CNC collet and was using it like a router collet. After calling tech support, I didn’t realize the internal cone snaps hard into the nut. Almost locks together. I was slipping it together as separate pieces. Once I snapped them together before installing, my alignment issue was totally gone. Just my rookie mistake. Maybe not fully seated?
Sounds like you have the ER-11 collets.
I don’t have a spindle and use the Makita style which don’t snap in the way you describe. Hoping to upgrade soon.
