getting accurate, round holes by CNC helical boring

[secretspy]

What is the best technique for getting the most accurate, round holes using a CNC end mill? (I cannot get my spindle slow enough for straight drilling, minimum is 10k rpm, so I am milling them.)

I am using my home-built 3-axis CNC router (gantry style mill) to bore some holes in aluminum, so that steel pins can be inserted and used to accurately position the stock for 2-sided ops.

I am finding that the holes are not coming out exactly round -- they are slightly ovalized, but not purely in X or Y. The long axis of the holes are at approximately NE / SW, maybe biased more towards Y (north/south). They also seem to be slightly tapered, with a smaller diameter at the bottom of the hole.

I've set up the toolpath to use a .125" 2-flute cutter to helicaly bore a .253" diameter hole, .350" deep, with a pitch of .020". According to my harbor freight calipers the pins are .248" diameter and 1.000" long. I'm using 15,000 rpm, 45 inches/min, which results in .0015" IPT.

On the first attempts, I tried climb-boring the holes using 2 passes with a .020" stepover, with a 3rd spring-pass. On the spring pass you can still hear it cutting, mostly as it gets to the bottom of the hole. Result: The pins go into the holes, but as the pins go further in, its more of a press-fit. There is a slight amount of play in the NE/SW direction, but tight in NW/SE.

On the 2nd attempts, I changed the toolpaths to do the first climb-boring pass leaving .006" of stock. and the 2nd climb-boring pass clearing that at the same speed. No spring pass. Result: Pins would not go in, but you could still see that the holes were ovalized in NE/SW. I could hammer them in, but that's not what I want.

This seems like the cutter is probably being pulled into the material at NE/SW due to different machine stiffness in X and Y. Or maybe its being deflected at NW/SE. Is there a different technique that would hopefully result in rounder, more accurate holes? Do I need to do a conventional pass and then a climb pass? Do I need to go faster to account for chip thinning? Slower to reduce deflection? Higher RPM? Full-depth finish pass? Please steer me in the right direction.


Other notes:

• I have checked the squareness of the X gantry to the Y rails by boring 3 holes a few inches apart in a triangular pattern, and pounding pins into them. Then, placing my machinist square on the pins, and checking for gaps with feeler gauges. A .0015" feeler (smallest I have) will not go between the square and any pin. It's as square as I can get it.
• I have trammed my spindle as good as I can get it using a dial-test indicator mounted in the spindle. It's within .002" over a ~4" span in both directions
• My spoilboard has been faced-milled to machine-level. No detectable sawtooth or trough pattern, which confirms tramming is good.
• I have adjusted the Z axis rails perpendicularity to the bed, by using the same dial-test indicator and running it up and down on the machinist square. It's within .003" over the entire 4" Z travel. Difficult to adjust and requires removing the carriage, re-assembling, and re-checking.
• There is no detectable backlash in any axis, checked with a dial indicator. It might have .001", hard to tell, the dial indicator was cheap. My machine has leadscrews in all axes, with delrin anti backlash leadnuts, and each leadscrew is clamped in a 2-bearing setup at the end opposite the motors, using delrin threadclamps against the bearings.
• Steps/unit is spot on. Calculated to be exactly 10,000 in all axes, with the microstepping and leadscrew pitch that I have. Checking it with a tape measure and a V-bit over 22" in X and 7" in Y confirms it.
• I tried turning on backlash compensation in Mach4 anyway, up to .005" in the Y axis, and it seemed to reduce the ovalization, but did not eliminate the it. I am hesitant to go any higher with that setting out of concern that it may cause other milled features to be inaccurate, especially in softer materials.

Similar Threads:

• How do you accurate mounting holes for SBR20 linear bearings?
• Drilling accurate holes in Al
• How to drill VERY accurate holes?
• Drilling VERY ACCURATE holes in delrin
• Helical Boring Help

[secretspy]

Here are the 3 pins I used to check squareness. You can see a small gap between the pin and the hole in the NE/SW (1:00 to 7:00) orientations.

[skrubol]

Not sure about the oval issue, but as far as the taper, .35 is pretty deep for a 1/8" mill, and will start to get a little bit of deflection. How long are the flutes? Stickout from spindle? Can you go up to a 3/16" end mill? For the same flute length and stickout you'll get 3x the stiffness (though there will be more force as well.)
You might try doing the undersize boring, then do a full depth contour followed by a spring pass contour.
Any way you could do a second op and ream these on a drill press or something?

[secretspy]

Not sure about the oval issue, but as far as the taper, .35 is pretty deep for a 1/8" mill, and will start to get a little bit of deflection. How long are the flutes? Stickout from spindle? Can you go up to a 3/16" end mill? For the same flute length and stickout you'll get 3x the stiffness (though there will be more force as well.)
You might try doing the undersize boring, then do a full depth contour followed by a spring pass contour.
Any way you could do a second op and ream these on a drill press or something?

All good suggestions, thank you.
The 1/8" endmill I'm using has 0.5" flutes. These cheapo ones:
https://www.ebay.com/itm/5-1-8-1250-...oAAOxyIAZRsSR-

I am inserting it into the collet as far as it will go, until the red plastic collar hits. So the total stickout is probably about 0.75". I don't yet have any 3/16" diameter endmills but that might be worth trying. I have a spot-drill than I can use to peck the center, and use the drill press to finish it. Don't have any reamers but maybe I need some

[skrubol]

Given that you're targeting 5 thou clearance, spotting or pre-drilling and drilling to size on the drill press should work fine, reamer might be overkill.

[secretspy]

I actually would like to target more like .001 or .002 clearance. I tried programming smaller holes in the tool path, but .253 seemed to be the smallest that the pin would go into. .251 did not work, not without using a mallet anyway.

[burbingus]

I don't have much experience with this type of machine, so take that into account. It sounds like you've pretty well checked all the backlash issues I would check first. I would also check any runout or slop in your spindle and make sure your collets were clean. Are you noticing any pull-out on your tool? Also:
-I would definitely run conventional for all operations removing larger amounts of material and only use climb milling for finishing cuts.
-To make the holes, I would try doing a peck drill operation first with a center drill then clean them out with the correct sized drill.

[hanermo]

Excellent post, unusually detailed and accurate and useful.

Imho.
As a professionally educated (haas) guy + 14 years experience.

IF your machine was actually accurate in terms of x-y linear axis stiffness, your results would probably be much better.
Your screws and linear guides are probably pretty much spaghetti. These are critical.
Your screw mounts are probably limp spaghetti. These are critical.

It is easy to test.
Mount wood bits around screw and clamp screw(s) to bed/structure via metal spacers.
How flexible is it ?

Most probable is that a fixed-screw clamped to frame is still very flexible (due to yoke + nut + screw too small) and the screw mount is very flexible and the yoke is very flexible.
Per axis.
And the bearing system is crap on all cheap mounts.

--
Re: the question, interpolate undersize 0.3 mm, ream to - 0.020 mm, then ream to 0.00 mm.

It is likely to be pretty good, and better needs stuff addressed above.

[ger21]

My machine has leadscrews in all axes, with delrin anti backlash leadnuts, and each leadscrew is clamped in a 2-bearing setup at the end opposite the motors, using delrin threadclamps against the bearings.

You do have backlash, and probably flex in your machine.
If you have the spring loaded nuts, they are really only zero backlash up to about 15lbs of load. With holes so small, the machines is rapidly changing direction, which will easily flex the spring loaded nuts.

Put a dial indicator on the tool, and push the collet nut with your finger. See how much it moves.

The reality is that you need a LOT of rigidity to cut perfectly round holes. One thing that might help is trying to cut a lot slower, maybe 10ipm, which should reduce the loads on the machine, and make it more accurate.

[secretspy]

Thank you all for the suggestions. I will try some of these when I get a chance.

To get down to 10ipm feed, I will have to use a 1-flute cutter at my minimum 10,000 rpm, resulting in a .001" chip load which I think is the minimum I would want for aluminum.

Sent from my Pixel using Tapatalk

[secretspy]

Success! I re-measured my pins and today they are measuring exactly .250". ($15 Harbor Freight calipers, I don't expect a lot from them)

Parameters that worked:

1-flute 1/8" cutter
10,000 rpm
10ipm ramp feed rate

Helical path with .010" pitch
Full depth .010" stepover finishing pass @ 13 ipm feed
Spring pass @ 13 ipm feed

Programming a .253" hole produced a uniform, slip-fit hole. Exactly what I was looking for.
Programming a .2525" hole produced a press-fit hole that required the pin to be hammered in. Removing the pin, I could hear the satisfying little "pop" from the suction effect, and I can see 4 places around the hole, 90 degrees apart, where the pin is making contact and pushing material out of the way. So I suppose its still not 100% round, but good enough for me.

I think I've pretty much found, and am playing near, the accuracy limits of my machine. The .2525" hole SHOULD still be a slip fit, but its good enough for what I'm doing, especially considering the dirt-cheap ebay cutter I'm using. And the fact that I changed the diameter by half a thousandth of an inch and could see a tangible difference, using a machine that I designed and built myself, makes me very happy

[skrubol]

That's great that you're getting so close (close enough it sounds.) Might be able to improve a little more with backlash compensation (if you haven't gone down that road already.)