[smokediver576]

Looking to press fit some steel bushings into 6061 aluminum. The bushing is approximately .500" in diameter x .500" in depth I need this to be a secure fit and not come out. What are folks suggestions?

My plan would be to pre-drill and then walk a contour cut in to the perfect fit.

Thanks,

[Jim Dawson]

Is this a through hole? Drilling and reaming to 0.499 or 0.4985 would be my choice, maybe a bit of bearing mount LocTite for added security. You could interpolate the hole if your machine is up to the task.

[smokediver576]

Is this a through hole? Drilling and reaming to 0.499 or 0.4985 would be my choice, maybe a bit of bearing mount LocTite for added security. You could interpolate the hole if your machine is up to the task.

Nope, it's not a through hole. I will already have the part set up in a fixture to run some of the other ops so I was thinking I could run it at the same time on the PCNC 1100.

[motoeng]

Looking to press fit some steel bushings into 6061 aluminum. The bushing is approximately .500" in diameter x .500" in depth I need this to be a secure fit and not come out. What are folks suggestions?

My plan would be to pre-drill and then walk a contour cut in to the perfect fit.

Thanks,

Are you looking for suggestions on what the AL diameter should be? I have access to ANSI B.41. If you want me to take a look at the suggested diameter for your application, let me know.

[Jim Dawson]

If you know how your machine does holes you should be good to go. I do it all the time on mine, but I know exactly how it's going to cut and compensate for expected errors with appropriate offsets.

[philbur]

Looking to press fit some steel bushings into 6061 aluminum. The bushing is approximately .500" in diameter x .500" in depth I need this to be a secure fit and not come out. What are folks suggestions?

My plan would be to pre-drill and then walk a contour cut in to the perfect fit.

Thanks,

Loctite. Otherwise I think you are into reamer tolerances and bushing diameters to + or - a tenth or so. You will never contour mill the hole to the necessary accuracy.

Phil

[smokediver576]

Newbie thinking out loud here..... The steel bushing is .499" - wall thickness on the bushing is .062" - I'm thinking steel into soft 6061... a little retaining compound.....

[Steve Seebold]

In the past, I have reamed the hole .0005 undersized then put the bushings in a solution of dry ice and acetone. Then the bushings would almost fall into the hole.

[RussMachine]

I would bore the hole .002 under the bushing size.
Leave the bushings in the freezer overnight, and warm up the Aluminum in the oven for a half- hour.
They should go together easily.

[philbur]

Newbie thinking out loud here..... The steel bushing is .499" - wall thickness on the bushing is .062" - I'm thinking steel into soft 6061... a little retaining compound.....

There you go. You need to press the bushing in straight or you may bell the aluminium hole. Use a vise or better still use the mill with a guide spigot in the spindle and the bushing and while the spindle is still lined up with the hole. If the bushing just drops in the loctite will do the job.

"Walking" a profiling cut in to the correct press diameter diameter requires accurate measurement or a go no go gauge. A slightly under-size bushing would do the job of a go no go gauge. Do you have the necessary measuring equipment and/or a lathe. If the measurement/gauge is not available then profile to a slip fit and loctite.

A profiled hole may be out of round by more than the required press fit tolerance. So again - loctite.

Phil

[smokediver576]

There you go. You need to press the bushing in straight or you may bell the aluminium hole. Use a vise or better still use the mill with a guide spigot in the spindle and the bushing and while the spindle is still lined up with the hole. If the bushing just drops in the loctite will do the job.

"Walking" a profiling cut in to the correct press diameter diameter requires accurate measurement or a go no go gauge. A slightly under-size bushing would do the job of a go no go gauge. Do you have the necessary measuring equipment and/or a lathe. If the measurement/gauge is not available then profile to a slip fit and loctite.

A profiled hole may be out of round by more than the required press fit tolerance. So again - loctite.

Phil

Hey Phil,
Yep I've got gauge pins to do the fit checking. My plan is to turn down a bushing insert tool on the lathe, put that into a TTS holder and have the mill press the bushing in about 1/3 of the way as part of the mill op on the part. I can then finish the pressing in over on the arbor press (5 ton).

Thanks for all the advice and help folks! I love this forum.

[GLCarlson]

Only thing I'd add is, "green Loctite". That is, 648, "press/closefit" Loctite. A new one on me, Tormach recommended it for a fix.

The proliferation of flavors of Loctite is either brilliant marketing with no real difference, or genuinely functional. I'm inclined to some actual functionality- the green stuff seems very runny, which is what one would want for press fits. I'd expect other flavors to work fine, though.

[IMT]

If you want to do it right. Look up the correct press fit value in a the Machinery's Handbook or other reference book. There are different classes of press fit and the amount of interference will vary with the diameter and materials involved. Once you determine the hole size, buy the correct reamer (they are available in .0001 increments from MSC or other suppliers).

[SCzEngrgGroup]

You will never contour mill the hole to the necessary accuracy.

I find that confusing.... Since I've done exactly that literally hundreds of times with absolutely no problems.

Regards,
Ray L.

[AUSTINMACHINING]

Drill/bore .005 under size, ream .001 under size and press fit. If you don't have excessive back lash and a fairly tight machine, you could get away without reaming and just helical bore. Dowel pins are cheap, just test on some scrap to dial in the process.

When reaming, half the speed and double the feed.

[philbur]

I find that confusing.... Since I've done exactly that literally hundreds of times with absolutely no problems.

Regards,
Ray L.

Well done, but not very helpful. Procedure?

Phil

[SCzEngrgGroup]

Well done, but not very helpful. Procedure?

Phil

No real procedure. Do a test piece to fine-tune the final diameter, as it will be affected by temperature, the specific tool, etc, but I just interpolate the hole, with multiple finish passes, then run a bunch of parts.

Regards,
Ray L.

[MechTec]

First you will need to be able to accurately measure the bushing diameter and the hole you are making. There is no need for more than .0005" interference fit for this bushing. If you are profile cutting the hole with your machine there is a way to get a little better roundness from the interpolation. Rough the holes out then go back and finish then with a .004" pass in both directions ( clockwise and counter-clockwise) leaving the tool size over its actual diameter by .002"and creeping up by adjusting the offset by .0002" to .0004" each time until you get to a diameter that is acceptable. It is important to drive the hole in both directions to achieve a "rounder" hole and it will help with position as well. Short of reaming or boring this will suffice for what you need to do. Hope this helps.

[philbur]

No real procedure. Do a test piece to fine-tune the final diameter, as it will be affected by temperature, the specific tool, etc, but I just interpolate the hole, with multiple finish passes, then run a bunch of parts.

Regards,
Ray L.

How did you evaluate the impact of the blind hole out of roundness on the ability to hold the bushing in place when in use.

Phil