interferance fit on small parts... tollerance help

[USAeng]

First off I hope I put this in the right section of the forum...

I looked up the tolerance in some iso charts online for parts .484" in diameter (shaft/hole) that will have interference press fit...

I found on the chart that the tollerance should be between 0 and 1.2 or so thousands for the interferance fit

So I specified the hole to be .4840 +.0000 -.0005 and the shaft to be .4840 +.0005 -.0000 so the interfernce will be right in the iso tollerances

The machinist asked how he could possible measure this... I told him to use his micrometers... he kinda scoffed and said he will make it to looser tolerances and get it to work...

I just wondered if there is a better way to do this that everyone could agree with?

Thanks.

 

[BrianE22]

Assuming the hole and shaft diameter are easily accessible, a micrometer would be fine for measuring the shaft diameter. A bore gage would be good for the hole. Both are very standard instruments - your tolerances are not extreme.

 

[USAeng]

Do the measurements and tollerances seem right for an interferance press fit? Thank you for the confirmation I was right about being able to measure that amount with regular machine shop tools... the guy made it sound like I was nuts... I guess he never goes over .001

 

[saberblue]

Check the Machineries Hand Book -- some one in the shop will have one other wise buy your own -- it is a great source for this kind of info

 

[MiketheEngineer]

The machinist might be testing you... Or it may be time to buy a new machinist

 

[USAeng]

I did use the machinist handbook too... but I found the iso numbers online first... I cant remember what it gave for numbers, but I think it was about the same...

The machinist is not testing me... he was being serious... unfortunately.... because I was pretty sure measuring those dimensions should not be a big deal...

So basically you guys are telling me to keep my dimensions and tell him to learn how to measure ?

 

[unclesyd]

Here is a Treatise on shaft design including interference fits.
There is a lot of information starting on Adobe page 38.

https://highered.mcgraw-hill.com/sites/dl/free/0073121932/365766/chapter07.pdf

The link should work, if not copy and paste.

 

[USAeng]

cool... thanks for that link... I remember using the H7/p6... I will read it completely today to see if it contains anything I may have overlooked. Thanks!

 

[USAeng]

great...

I went over everything again a little more and changed it a little using the materials you gave me in that last link... my dimensions are now

Hole: .4840-.4847
Shaft: .4847-.4851

I am a little confused on the definitions of "type of fit" as in table 7-9 on page 385 in that link.... as of now I am using an interference fit H7/p6. From what I can gather from the description it is what I want.

I want to put the shaft in the hole and have it so the shaft does not move and it wont come out... Is there someone that can describe a little differently the descriptions of the "locational transition fit" H7/k6 and H7/n6?

It seems when I do the math that there would be a chance of it being able to come out in service if I used at transition fit H7/n6 as the hole would be .4840-.4847 and the shaft would be .4845-.4849

Thanks a lot!

 

[MikeHalloran]

You don't really have a guaranteed interference fit. You will be able to push the pieces apart by hand if the hole and shaft both happen to be the same size. If you want to have a true interference fit, you need to provide inteference at all material conditions, i.e. the smallest allowed shaft has to be a few tenths bigger than the largest allowed hole.

I'm not sure what your machinist was trying to say. It appears that he intends to make one part to somewhere near the nominal size, and make the other part to fit. Which is fine, if you don't need the parts to be interchangeable.



Mike Halloran
Pembroke Pines, FL, USA

 

[USAeng]

ok cool... thanks for the input... at least for the drawing I will decrease the tollerance on the hole .001 to make sure there is an interference at all conditions... it is strange that those calculations in the book still show that if the parts are exactly the same dimension that it is an interference fit... I will talk with the machinist to make sure he makes something that will work, but at least this way if we ever send the drawings out to be made somewhere we will be safe.

Thanks a lot for all the input

 

[MikeHalloran]

Be careful throwing .001s around. For small holes and press fits, that's a big change. An interference of a couple of tenths would be fine. It might be helpful to go through the calculations for press fit force that you will find in, e.g., Machinery's Handbook. If you don't have one of those, go buy it; it's the one book you need.



Mike Halloran
Pembroke Pines, FL, USA

 

[ajack1]

I totally agree with Mike on that, a potential interference of .0019 on a hole that size is a serious amount.

 

[juergenwt]

Go here and scroll down about 1/2 way for FITS:

http://www.mitcalc.com/doc/tolerances/help/en/tolerancestxt.htm

 

[USAeng]

whoops... meant .0001 not .001

 

[desertfox]

Hi USAeng

Your machinist might have point about how to measure to 0.0005 unless his micrometer as a vernier scale on it, as an apprentice my micrometer was accurate to0.001", see this link:-

http://en.wikipedia.org/wiki/Micrometer.

Secondly you don't say what your application is but normally an interference fit would be selected on service conditions ie external loads or torque, thermal expansion of parts etc.
Can you give us anymore detail?

desertfox

 

[USAeng]

His has a vernier on it...

I did try to explain the fit a little above... I guess I have a hard time describing it because there are no requirements other than it cant come apart. It doesnt have any specific load/torque on it is part of a nozzle that could not be made out of one part as all the angles made it too difficult to make therefore they wanted to make it out of two and join them together. They said that an interference fit would be best and so I looked up the appropriate dimensions and put them on the dwg.

 

[turb1]

The tolerances that you have are not excessive to the right machinist. In my experience, it depends what the machinist's background is. It is common for some parts to have extremely tight tolerances (I have worked with some high speed bearing applications in the 1-2 inch diameter bore range the overall tolerance is plus .0002 minus 0). These parts are made on "normal" machining equipment with machinists who are used to holding these kind of tolerances.

Also, a line to line fit is not necessarily bad, it depends on the engagement of the shaft and the loads applied to the part (if any).

 

[BillPSU]

If this is a production job get the appropriate equipment to gauge these tolerances. A micrometer with a vernier is appropriate for a short run job but be warned .0005 is the smallest I would be comfortable gauging with a standard micrometer. If this is a long run job get a dial bore gauge with a ring standard and an indicating micrometer or snap gages to measure the OD.

Getting the correct "feel" with a micrometer is the problem. If you don't believe take a micrometer out to 3-4 machinist with a sample part and as them to measure the part at one specific point within .0001. You will be surprised by the variation.