[Bryan Turner]

So I have a job coming up with high(er) accuracy than usual (needs +/- 0.001). I made some test pieces and they were all off by about 3-5 thou in various dimensions. Decided to go back to basics to get a baseline before trying any adjustments. I cut 5 "squares" out of aluminum with commanded size of 0.75". Cut path was a contour with helical descent, followed by a 0.005" full-depth cleanup pass. Photo attached.



Results are very consistent, so that's good. Along the top edge, in both dimensions, the size is 0.754-0.755. As you move deeper into the cut the size moves out to 0.758-0.759. I need to bring these down to 0.750-0.752.

It was leveled and trammed but otherwise unadjusted since installation about 4 years ago. Rarely need precision parts, so I don't have any records of accuracy back then. I know it's not backlash, since I regularly watch my Haimer during part setup and it's always around 0.001. The machine is due for a thorough maintenance anyway, so this seems like a good time to delve into the accuracy issues as well. Anyone have a punchlist for tracking this down?

Searching recent posts, this is what I have so far:
- Check gibs
- Check runout
- Check tram & level
- Check slideway racking
- Check twist in base
- Test cut an ID or OD circle, then check for out-of-roundness (from Keen's thread on accuracy)
- Just realized I should have put a fresh cutter in to eliminate cutter wear, but 0.0025" cutter wear seems implausible (3/8" 3fl HSS).

Thanks,
--Bryan

[CountrySmith]

For cutting external geometry, I would expect lost motion to give a smaller than nominal dimension. It would appear to me that your running larger than nominal but the same in both x and y could be caused by tool deflection. The fact that your dimensions increase as you go down the block would support that.premise. I would try again with a new end mill.

To determine whether this is a cutter problem or a problem with the mill, you could sweep a 1-2-3 block with your Haimer as a test. You will have essentially zero deflection force that way. You could also mill a rectangular pocket and check the dimensions that way. If cutter deflection is the cause, you will see smaller dimensions.

RJ

[flick]

Since your machine is repeating, the accuracy you're looking for is easy to obtain if you can straighten out those walls.

CountrySmith is right - all signs point to deflection. The deflection may be coming partly from the cutter (switch to a sharp carbide cutter for best results) but from the sheer amount of taper in those walls, I'd say a Z axis gib adjustment is probably overdue.

[tmarks11]

How much stick-out did you have on the endmill, what is the diameter, and what was the DOC?

Also, are you sure you got the diameter of the endmill correct? a 0.5" endmill isn't always exactly 0.500". You can mic it to get close, and take a test cut to see if you are right.

[TurboStep]

Cut path was a contour with helical descent, followed by a 0.005" full-depth cleanup pass.

What speeds and feeds were you using?
Step

[RussMachine]

For accuracy, I would try using two tools, A rougher and a finisher.
Rough out 95% of the material with your roughing endmill, then just 'Skim' the walls with new, sharp, finishing endmill.

[Bryan Turner]

> You could also mill a rectangular pocket and check the dimensions that way

Yes, the first test pieces had pockets too small and outer profile too large. I decided to start with fixing the outer profile since I have more precise measuring tools for that.

> sweep a 1-2-3 block with your Haimer

Did a quick test, zeroing the Haimer at the table then measuring the height of a 1-2-3 block turned to each of its sides: 1.0027, 2.0023, 3.0023
Not sure if you're referring to sweeping along the X/Y axis though?

> all signs point to deflection
> Z axis gib adjustment is probably overdue

Thanks, sounds like a good direction to go.

> How much stick-out did you have on the endmill, what is the diameter, and what was the DOC?
> What speeds and feeds were you using?

0.375" nominal diameter, 3 flute, HSS
Overhang is about 0.8"
0.05" DOC
0.375" WOC
6100 RPM
42 IPM

Here's a link to these settings already entered into my Speeds & Feeds Calculator:
3/8" 3fl HSS in Aluminum

It's a 3-flute end mill, so I'm not exactly sure how to measure the diameter at the flutes directly. I read something about rolling the end mill on a granite stone measuring the height of each flute?

> For accuracy, I would try using two tools, A rougher and a finisher.

I'll mount a new carbide end mill and use that for the finish pass.


Thanks all, looks like the first order of business will be the Z axis gib.
--Bryan

[chuckorlando]

Spring passes. Run the last pass twice.

[tmarks11]

0.375" nominal diameter, 3 flute, HSS

When your geometry permits, the largest diameter endmill is going to give you the least deflection.

0.05" DOC
0.375" WOC

You are cutting the exterior of an aluminum block, with a WOC equal to the diameter of your endmill?

For side cutting, usually keep your WOC at 20-30% of the diameter of your endmill (never exceed 2/3 of diameter), and take a much deeper cut than 0.050". Your endmills will last much longer if you use most of the flutes when side cutting instead of just the tip. To prevent deflection, just keep your WOC down.

Doing a side cut at 100% the width of your endmill is going to give you deflection and/or chattering issues (like you would normally expect from slotting).

[MichaelHenry]

It's a 3-flute end mill, so I'm not exactly sure how to measure the diameter at the flutes directly. I read something about rolling the end mill on a granite stone measuring the height of each flute?

There are V-anvil micrometers that can be used to measure end mill diameters with odd numbers of flutes, but they are pricey, even used. Shars has some pretty decent prices for new. Their quality on some products can be spotty but they've been good to me about accepting returns with no hassle. The V angle is important to get right, I think. Different angles are needed for 3, 5, and 7 flute end mills. End mills with even-numbered flutes can be measured with a standard micrometer. If it helps, I've noticed that my 8-year old 1100 usually mills rectangular bosses a little oversize, too. I put that down at least partially to end mills being generally a little undersized.

SHARS .2-.8" Electronic V-Anvil Micrometer NEW | eBay

Please post an update with your results. I, for one, would really like to see that.

[Uman]

Apparently new endmills vary slightly in diameter for a given size and measuring with a mic is not always super accurate in my hands. So I have used this method: mount a block of aluminum in the vise, clean up both opposing sides, measure and cut about 20 thou or so off each side again at 1x dia DOC. Measure and adjust diameter offset. Repeat.

[Steve Seebold]

Spring passes. Run the last pass twice.

I always do 2 spring passes when I cut aluminum on my 1100.

I've always been able to hold +/-.001 all day on my machine.

[Bryan Turner]

Thanks all, good comments. Looks like the Z-axis gib was the right diagnosis.

When I went to adjust the gib, I loosened the upper retainer 8 turns, but the lower retainer would only tighten 3 turns. I also noticed the upper retainer washer was not in the circular alignment slot of the dovetail (before unscrewing), so backing it out 8 turns made the screw floppy. Decided to start with just 3 turns and go from there.

Going through the adjustment procedure, my gib is now WAY lower (~8 turns) with both retainer washers settled into the alignment slots. Seems I've been running with essentially no gib contact on the Z axis. During the original installation I did check that all the gibs were tight, but did not measure their position. Backlash was well within spec, so I had no cause to discover this mis-adjustment.

After adjustment, Z backlash basically hasn't changed: 0.0011"

> When your geometry permits, the largest diameter endmill is going to give you the least deflection.
> You are cutting the exterior of an aluminum block, with a WOC equal to the diameter of your endmill?

The actual parts will be profile cut, yes. The test pieces (shown in the first message) were milled out of some scrap plate using a helical slotting operation, with 0.005 left over for a full-depth finish pass. If I understand correctly, the full slot operation may have had significant deflection, but the finish pass to bring the part to size should have negligible deflection.

I don't use end mills larger than 3/8" due to low torque (except the shear hog), so I'm limited in the short term to test with those. However, I will switch to carbide to reduce the flex.

> Spring passes. Run the last pass twice.

I added that to my test cut procedure:
- Fresh carbide cutter
- Measure actual cutter diameter
- Rough with different end mill
- Finish pass
- Spring pass

My only fresh carbide cutter was a 3/8" 3fl ball mill, so only the upper edge will give a valid measurement. I cut two new squares, running the finish pass twice using the fresh cutter. Results are much improved!

X axis is still a little off; 0.7522
Y axis is dead-on: 0.7504

Attachment 340056

Time to check Z-depth accuracy, and tighten up that X-axis. This gives me much more confidence on this job - should be able to run an example part again this week. Wouldn't want to hand-finish 600 parts..ugh.
--Bryan

[flick]

Time to check Z-depth accuracy, and tighten up that X-axis.

Congrats on your improved results. Bear in mind that the Y axis gib is the one that would affect sizes in the X direction.

[chuckorlando]

Sweet my man. Make that money

[Uman]

Spring passes. Run the last pass twice.

This seems like a rub pass that would reduce cutter life, but would indeed jazz up the finish.

[TurboStep]

1. - Fresh carbide cutter
2. - Measure actual cutter diameter
3. - Rough with different end mill
4. - Finish pass
5. - Spring pass

I agree with Uman. A spring pass just handles the symptoms without correcting the underlying issue (5. - Spring pass).
Your original post indicated a taper of 0.004, or 0.002 per side. If I estimate these measurements to have been taken maybe 1/4" apart this would indicate that something is flexing at around the same distance above the part - i.e. 1/4" above the part (very roughly). I can't imagine how the Z-axis (gib) could be responsible for this. I would be much more inclined to suspect tool flex. I asked earlier about the feeds and speeds because a slow finishing pass can easily rub and push the tool away from the work-piece, much more than flex estimated from normal cutting forces. I assume the feeds you quoted were only for the roughing, but if you're using the same values for finishing as well the taper may simply be due to rubbing if cutting edges of the flutes are partially worn (blunt) or even broken at the tips. If the feed for the finishing pass is too slow even a new tool will rub and holding tolerances will be difficult.
I've never come across any cutters with more than a couple of tenths (thou) under-size. Unless your cutter has been re-sharpened this difference should be insignificant compared with the errors you're experiencing (2. - Measure actual cutter diameter). I measure my 3 Flute end mills using a dial vernier with 0.01 mm resolution. I can measure multiple flute "peaks" along the length and compare the measurement against the shank diameter (verified with a micrometer) or a slip gauge. I wouldn't normally need to do this because of the expected runout:
The runout is likely to be larger than the diameter error and the result will oppose any cutter under-size i.e. will reduce the size of any external dimensions.
Roughing with a different end mill (3. - Rough with different end mill) won't improve the tolerances providing the mill you use for finishing is still good. Reserving specific end mills for finishing only will simply increase their useful life - unless you do too many spring passes
One finish pass (4. - Finish pass) is all you should need to obtain sub 0.001" tolerances.
Recipe: Check the cutting edges (1. - Fresh carbide cutter) and keep the feed rate up in order to maintain a suitable chip load. It doesn't have to be carbide for a 3/8" and 0.8" overhang.
Step

[Bryan Turner]

> A spring pass just handles the symptoms without correcting the underlying issue

Definitely want to correct the issue!

> 0.002 per side .. maybe 1/4" apart .. indicate that something is flexing at around the same distance above the part
> I can't imagine how the Z-axis (gib) could be responsible for this.

Hmm.. this is a good math question!

Part is 1/2" aluminum bar, test cut was down to 0.45, leaving a 0.05 tab to cut off. I measured with micrometer from "middle of anvil at top edge of part" down to "bottom of anvil just above the bottom of cut". I avoided measuring directly at the bottom of the cut since the used cutter's corners might have some measurable rounding. Not sure how wide the anvils are, but I'd guess 1/4".

So I'd estimate the total measurement distance is 0.44 - 0.125 = 0.315. Depending on where the fulcrum is placed we might find different amounts of misalignment.

If we assume the head is perfect and tool deflection is the only force, the fulcrum would be at the tool holder interface, 0.8" above the bottom of the cut. For a 3/8" HSS end mill, it would require ~307# of force to deflect the end mill by 0.002" (force to deflect 0.002"). Tormach reports the steppers have approximately 200# of force (can't recall where I read this at the moment), so it seems implausible that the machine would be able to bend the endmill that far. So, since there was no grunting from the steppers and the cut sounded smooth, I surmise that the fulcrum must be higher up.

[edited]
If we assume the fulcrum is in the middle of the Z gib then we need to find the slop in the Z gib to make the same angle as the taper on the part. A taper that generates 0.002" of misalignment at 0.315" is 0.36-degrees. If we guess the length of the gib to be 8" (wild guess), this would mean we need ~0.05" of slop along the length of the gib to cause the taper.

I think that sounds plausible considering that my gib appears to have been totally disconnected from the z-axis!

> I asked earlier about the feeds and speeds because a slow finishing pass can easily rub and push the tool away from the work-piece, much more than flex estimated from normal cutting forces.

Sorry, didn't report the finishing feeds. It turns out that the finish feed is the same as the slotting/roughing feed, since the slotting is very low DOC and wide WOC, while the finish feed is low WOC and high DOC (finish feeds & speeds).

Of course, I did not update the g-code on the last test cut to the proper speeds & feeds for carbide, so your comment is totally valid. My last good 3/8" carbide tried to eat a SS bolt at 0.5 DOC and 35+ IPM. Needless to say, its eyes were bigger than its stomach.

> The runout is likely to be larger than the diameter error

Yes.. didn't measure runout yet. I'll add that to the list:

- Rough with different end mill
- Fresh carbide cutter
- Measure runout
- Finish pass
- NO Spring pass (don't cover up a problem if we're trying to correct it)

Should have time tonight to try the X/Y axis adjustments.

Thanks all!
--Bryan

[TurboStep]

If we assume the fulcrum is in the middle of the Z gib then we need to find the slop in the Z gib to make the same angle as the taper on the part. A taper that generates 0.002" of misalignment at 0.315" is 0.36-degrees. If we guess the length of the gib to be 8" (wild guess), this would mean we need ~0.05" of slop along the length of the gib to cause the taper.

So if we take the distance from the middle of the gib to the tool and assume the head, tool holder and end mill are tilted at 0.36 degrees, how much larger would you estimate your part to be ??
Step

[cncoperator]

>
. Tormach reports the steppers have approximately 200# of force,,,so it seems implausible that the machine would be able to bend the endmill that far

How does approximately 200# (in-lb? ft-lb?) at the stepper relate to force at the cutter...?