What's new
What's new

Tolerance on hardened sleeve for press fit

maxwellhouse

Plastic
Joined
Apr 17, 2020
I am new here but hope this is the right spot to ask but I am newer engineer in the design aspect auto industry.

I am working on a project for a press fit sleeve and wondering if the tolerance I need is going to be crazy or if anyone here with some experience can give some insight.
Essentially the part is a 1045 tube, 1.75in long, ID .830 nominal, OD 1.00, HRC 45 and a surface finish on the OD of ~95Ra. (All converted from metric but close enough for me)
My main concern is the tolerance I need on the ID of +-.001in/ .05mm along with the thinner wall thickness

This part would be ~50k parts a year and I'm hoping someone with some production experience can tell me if someone could hold the ID tolerance with the volume somewhat easily or if it would be a struggle.
That is the tolerance I need and I'm trying to see how bad the cost impact for this is going to be because I know tight tolerance=high price.

Thanks in advance for any help or insight
 
Only negative I can see is tubing is really not very round, so you might be fighting that. How much material will you be removing from the ID? Starting from solid bar may be a better option.
 
Your cut procedures will come into play so you can hold concentricity. Working offsets and dealing with tool pressure will also come into play.
 
Your question is about holding a +-.001" tolerance!! I wish, that's gravy for me. I'm not bragging just making a point that it wouldn't even cross my mind as something to struggle with. Assuming you're not working on a complete POS Lathe. I agree making it out of solid, will be way easier.

R
 
I think this is quite doable with the right tooling. With a .085" wall, the shop that makes these is not just going to toss some tubing in a 3-jaw chuck and bore it out, but it shouldn't be a very exotic procedure. When manual turret lathes ruled the Earth, this could have been done with tube stock of "sufficiently" oversized OD and undersized ID to ensure eccentricity from cheap chucking would clean up OK, then both OD and ID would have been roughed simultaneously with a preset tool having two inserts, then finished with a second preset tool, and parted off.

What's your concentricity tolerance? There are a whole bunch of final sizing techniques from ball burnishing to broaching that might work, but they don't do anything helpful to put OD and ID on the same axis. Cutting OD and ID simultaneously, as described above, more or less guarantees good concentricity and balances out most of the cutting forces that would tend to deflect the part and develop tapers.

If your part were substantially longer, then other approaches might have to be taken. But +- 0.001 is not a tough requirement. +- 0.0001 is another matter.

[Added in edit] If it were me, I would be calling for a rather tighter tolerance. 0.001" interference per 1" is a rule of thumb, but it tends to lead to hard press fits, certainly hard enough to expand a tube with 0.085" wall. In the absence of other engineering constraints, on a 0.83" ID, I'd start by asking for +0.0000 -0.0005 with the nominal size 0.0005" less than your shaft size. And obviously the shaft diameter has to be closely controlled, too.
 
When talking about manufacturing a press fitted component, you'll need to simultaneously concern yourself with the sleeve AND the hole it's going into. The diameter of the hole and it's tolerances will have a direct impact on what your sleeve ID size is after fitment. If you're not the person in control of the hole your sleeve is going into, you'll need to find out who is and work this out together.

And as sfriedberg above was referring to a shaft possibly passing through this pressed in sleeve, you'll have to know what's going on with the shaft's tolerances as well. Possibly this information is already at hand.

In short, your sleeve will reach it's final size after it's pressed in. Your sleeve/bore drawing tolerances have to work together toward that end.
 
And then consider heat treat distortion and post heat treat finishing- 45Rc is going to require a quench and temper step and you are not going to be able to control anything near that tolerance by not finishing the ID after heat treat- probably hard turning is the least expensive- depending on wall thickness, you might ball burnish it. Honing and grinding is going to be more expensive.
 
Is the part sleeving into a hole or sleeving over a pin?

For the ID, if starting with tube, I'd get it close with a boring bar and finish with a carbide reamer. From solid, drill and ream, both carbide. Should be able to hold tenths all day long. From solid is probably faster.
 
Thanks for the input and advice everyone. Ill look into a few of the items but a few follow ups if anyone was wondering.
This is a press fit to go around a tubular shaft.

Runout is 0.01 so I don't think that would be a big issue and could probably be machined either at once or the same time

If the OD happens to stretch, it wont be an issue. The reason for this part is the mating shaft is to soft for a clutch/slip ring to slip correctly. If anything, I think we will compress the softer material rather than stretch the sleeve. The slip ring has a wide tolerence it will slip correctly. OD of the sleeve has a tolerance of +-.003

13engines and sfriedberg completely agree and that is my issue. I have the mating shaft but it will be a swaged tube that can only hold 3-4 thou. I'm just trying to play the balancing game between making everyone happy and not having outrageous press loads.

Thanks again everyone. It sounds like I wont make the machinist too upset with this.
 
If the OD happens to stretch, it wont be an issue. The reason for this part is the mating shaft is to soft for a clutch/slip ring to slip correctly. If anything, I think we will compress the softer material rather than stretch the sleeve.


Don't forget that within the elastic limit, Young's modulus does not change with hardness (heat treating). i.e. A heat treated part is no "stiffer" than a dead soft part, provided it does not exceed the yield limit.

PM
 








 
Back
Top