What's new
What's new

Bowed taper on 1" bore using 1/2" end mill on VMC

dardeshna

Plastic
Joined
Dec 10, 2015
I'm getting an odd wall taper when trying to walk in a bore for a needle roller bearing. The bore is 1.02" OD, 1.18" deep, and the wall thickness around the top 0.8" of the bore is only 0.15" (the part is a hub of sorts).

I'm trying to achieve a press fit of -0.0009" to -0.0015" on the diameter, however the best I could do was a "bowed" wall. At the top, it was -0.0002", in the middle it was +0.0004" and at the bottom it was -0.0018". No matter how I walked it in, the taper remained pretty similar.

Specs:
Machine - VF2SS
Material - 7075 Al
Cutter - 1/2" 3FL 2"LOC
Roughing Speed - 12K RPM, 72IPM, 0.002IPT
Finishing Speed - 5K RPM, 22.5IPM, 0.0015IPT

Cutting Strategy:
  1. Rough out to 0.02" radial stock remaining
  2. Finish to 0.002" radial stock remaining with 0.007" stepover, climb cutting
  3. Walk in to desired dimension using cutter comp (~2 attempts, climb cutting, spring pass on each)
What I think it could be:
  • Tool deflection: This the primary suspect in my opinion. The tool is 4x in length compared to diameter. This doesn't explain how the bore gets wider before getting narrower however.
  • Climb vs conventional: The general consensus seems to be that climb cutting deflects the tool perpendicular to the feed direction while conventional might help when finishing because deflection is long the feed direction?
  • Tool tip wear: I'm trying to break the habit of roughing at 1-1.5x DOC, 0.05x WOC, but maybe this is contributing to why the bore is smaller at the bottom.
  • Thin part wall: 7075 isn't the stiffest material and the part wall is only 0.15" for most of the depth of the bore. Perhaps the wall is deflecting at the top?
  • Feed rate / chip thinning: I've read that taking too shallow of a cut can cause the tool to rub and deflect more. I tried cranking the finishing feed rate up to 40IPM and then 60IPM on the second attempt, but it didn't do much other than worsen the surface finish.
What I don't think it is:
  • Tool runout: I'm using a hydraulic tool holder and the tool is relatively large so I don't believe runout should be a huge contributor. Admittedly I have not checked tool runout.
Possible solutions:
  • 3/4" end mill: I think this one is kind of a no brainer but I just ran out of time. I'd probably have to be more careful of slowing down the feed rate since it's getting close to the diameter of the bore.
  • Machine the bore first: If I machine the bore first before roughing the outside, then the wall thickness shouldn't be an issue. I do have a slight concern about the bore warping as the outside is then machined away.
  • Conventional mill: I'll give this a shot when walking in the bore and see if it helps the taper.
I'm going to do some more experimenting next time I'm in the shop, but I welcome any insight or theories. Is there something obviously wrong with my approach? Should I just cut my losses and find a boring head? I only have to make a few of these, but I also just want to become a better machinist :)
 
If you ever turned a part on a lathe without a dead center you may note that the unsupported end tapers slightly to a few thou larger than the end near the chuck due to the part bending away from the tool.
Maybe you're experiencing the same sort of thing where the relatively long cutter is deflecting outwards causing your taper. Try the shorter larger diameter end mill to see if the taper is reduced.
 
Take your tool and sharpen the flutes by hand. Do not sharpen the last .25 to .375 at end. No worry about how bad it looks, just reduce the OD (think Reduced Shank). Spiral in. You are getting tool deflection and switching to a .75 em will not help.
 
I'd quit trying to interpolate the bore.

We make a very similar part with about the same proportions, and the mass around the bore is unevenly distributed on top of it. Get a boring head with the biggest shank you can find and choke it way up in a 40 taper holder. Leave maybe .002 in the diameter and finish bore it. Round, straight hole, end of problem.
 
Best guess is your tool is tilted in an orientation where it have less runout in the middle than at the top and bottom. If this is true helixing down should show different results.

There are lots of machines that will interpolate a bore very well. To say always to bore holes is a blanket statement that doesn't always hold true. I have one machine that using a boring bar is a total waste of time, the rest of the machines struggle to hold better than a few tenths.

Know your machines and program accordingly
 
Best guess is your tool is tilted in an orientation where it have less runout in the middle than at the top and bottom. If this is true helixing down should show different results.

There are lots of machines that will interpolate a bore very well. To say always to bore holes is a blanket statement that doesn't always hold true. I have one machine that using a boring bar is a total waste of time, the rest of the machines struggle to hold better than a few tenths.

Know your machines and program accordingly

It wouldn't even have to be tilted. Endmills have helical flutes; if it's off center in the direction of the end of a flute, then that end will be further off center than the middle. If the top of the hole is at the distance where next flute lines up with the end, Bob's your uncle. So yeah, runout. And yes, helixing down will help to overcome that. Don't try to sharpen an endmill by hand, you'll ruin it.
 
There are lots of machines that will interpolate a bore very well.

It's not the machine accuracy, it's the process. The cylindricity of the hole is affected by deflection, axial misalignment of the tool shank, taper error of the endmill, or something as small as a nick in the flutes. All the above are eliminated by single-pointing.

But of course it all comes down to what the job demands (or whether the customer knows the difference). If it's your own product the needle bearing is going in, the stakes may be higher.
 
It's not the machine accuracy,

Sure it is, if the machine isn't rigid with high accuracy preloaded screws your hopes of a round bore are pretty slim despite how much backlash comp and pitch error comp you have

it's the process. The cylindricity of the hole is affected by deflection,

A few light finish passes will take care of that, and or a helix

axial misalignment of the tool shank,

shrink fit

taper error of the endmill

high quality endmills

, or something as small as a nick in the flutes.

time for a new tool, a nick in any finishing tool will produce an unacceptable condition

All the above are eliminated by single-pointing.

not really, backlash can cause the bar to push the table around causing an out of round bore

But of course it all comes down to what the job demands (or whether the customer knows the difference). If it's your own product the needle bearing is going in, the stakes may be higher.

I've never had a drawing call out the procedure to machine a hole, only the tolerances to machine it to. Though I'm sure it exists I haven't ran into it.

I'm not saying single point boring is bad, I do it often, but I can also interpolate a hole of the same quality and usually with a better surface finish
 
Try milling it as a helix. Say .080 stepdown per turn. Might also help to relieve the end mill so the flutes up top don’t push the bottom away. I have also seen where taking a pass that should cut say .0002” smaller... can allow the top of the cutter to be clear of the top of the bore allowing the bottom to cut to size. We have similar machines and while we try to use shorter tools than 4XD like you have here even then it works. Similar tolerances on smaller holes, even! You’ll get it.
 
Thanks for all the replies! I gotta make a few more of these hubs this weekend so I'll try helixing in and see if that yields better results. Luckily these are just some parts for our student project team so I've got some time to experiment.
 








 
Back
Top