Let's have a discussion on position tolerance of dowel pins

[yacpro13]

Hi guys,
I'm finally signed up as a member here on eng-tips. Been reading the forums for longer than I can remember, was great help through school and now graduated 1 year ago.

So I'd like to discuss about position tolerances of dowel pins.

For example, let's say we have Part#1 with two 0.250 dowel pins press fitted in it.
For Part#2, we want to locate accurately and be able to assemble and disassemble by hand; for this we select slip fits on the two dowel pin holes.

Now let's say I dimension my slip fit hole to be .252 to .253 (so .002 to .003 clearance on the dowel pin).
This would require the position tolerance on all dowel pins holes to be .001 on the diameter, which I though was reasonable for standard machining processes (milling, whether CNC or conventional).

When I released this drawing and the parts were manufacturer, the CNC manager told me that .252 reamers are not standard, and that a .002-.003 clearance was too much of a clearance. So I told him I could reduce the clearance and dimension my slip fit dowel pin holes to .251 to .252 (and I should say here that he thought this was still too much of a clearance), but that would mean that I would have to tighten the position tolerance to .0005, and I thought this was a way too tight of a position clearance than was reasonable.

So my question:
What is a reasonable position tolerance to put on on dowel pins holes?
What is an average position tolerance that can be attained on conventinal/CNC milling machines?

I found a lot of info on the fits for the diameters, but none on the position tolerance.

Thanks!

 

[fsincox]

You need to base it on the function, is this basically a one time assembly or does it have to assemble over and over without broaching out the holes. If the latter the tolerance will need to be very tight. The numbers you are mentioning are very close to what we used in the machine tool industry as standard.
In the shop I am in now, they whine and cry at twice the tolerance we used to require as standard in machine tools.

 

[cjccmc]

I agree with fsincox, the function should dictate the tolerance. And if the resultant tolerance is tighter than practical you can look for alternate solutions, which could be:
1. match drilling
2. use a slot for the second pin (clocking control)

I have seen designs that either lack or have incorrect tolerances yet the parts received from the shops fit together nicely. However, if you were to perform a worst case tolerance stack and revise the prints to show these it would raise some eyebrows

 

[cjccmc]

As to the possible values for tolerances I would not hesitate to go with POS dia .0005 feature to feature (i.e. hole to hole on one part and pin to pin on the other). Also, you will need to apply a projected tolerance value to the pin holes equal to the protruding height of the installed pin.

 

[fsincox]

Are you using a round and relieved pin combination or 2 straight pins?

 

[yacpro13]

@fsincox: I agree to base all these decisions on function. In this case, say function is locating, with the requirement of assembly and disassembling by hand (for maintenance). Say the parts will be assembled and disassembled say once a month.
In this case, the dowel pins are just 2 standard straight pins.

@cjccmc: Like you say, I have seen drawings too that, in the worst case, would not assemble. It was actually recommended to me to use that practise. It was suggested that I put .0005 clearance on the dowel pin holes on my drawings. I raise the point that this would require a position tolerance of .00025 (on the diameter!!) , to which I was answered, "at assembly,if it does not fit, we'll oversize the holes".
I like to know that the parts I design will fit together without requiring fiddling at assembly.

So the parts that I described above, with the two slip fit dowel pins holes of .252-.253, were manufactured, and the CNC manager has a point: when you mate the parts, you can move them one into the other a little. You definitely 'feel' the clearance of .002.

This suggests that I should follow his advise, and tighten the fit on the dowel pin slip fit holes.
As a result, this would also tighten the fit on the position tolerance. Without a reference frame as to 'how easy' it is to hold a position tolerance of .0005 on the diameters of the dowel pins holes, I'm relunctant to put that on my drawings.

Here's another (similar) question: what position tolerance on the diameter of dowel pin holes do you use in the case where the dowel pins are press fitted into both parts?

 

[fsincox]

I think generally, when using pins, the function is locating.
The key to me is: is it essentially a one time (basically, permanent) assembly or must it reassemble without a significant degradation over time (the pins broach the holes).
We had both in machine tool. Gear cases used dowel pins that were creating essentially permanent assemblies (vary rarely disassembled) the parts could be driven together at assembly.
We made transfer lines for all of the big car companies. Every single engine block sees every single machining station and was located on a face (primary) and 2 dowels (one round and one relieved). You do not want the location to get sloppier as it goes down the line so the tolerances are tight and must they be.

 

[drawoh]

yacpro13,

We are missing an important design procedure here.

One dowel pin engages an accurate, round clearance hole. The other dowel pin engages a slot that lines up with the first hole. Now, all your holes can be located to reasonable machining tolerances of Ø.010", you can use ultra accurate tolerances on the diameter of the round hole and the width of your slit, and the assembly will be very repeatable.

--
JHG

 

[fsincox]

drawoh,
I agree, though I would call that more of an alternate possible design option rather than any kind of required standard design proceedure.

 

[btrueblood]

I can't add much to the tolerance arguement. But this stood out:

"CNC manager told me that .252 reamers are not standard"

I call BS. Chucking reamers in 1/4" size are generally available from any good tool supplier in stocked increments of .0005", with tolerances typically +.0002/-.0000. See mcmaster catalog, MSC catalog, others... He may need to look under "oversized reamers" to find them in (for example) MSC catalog, but they do exist.

 

[drawoh]

fsincox,

There are three ways to do this.

[ol ]
[li]Clearance hole and clearance slot for dowels[/li]
[li]One round dowel pin and one diamond shaped dowel pin.[/li]
[li]Drill the dowel holes after assembly.[/li]
[/ol]

Pick one.

--
JHG

 

[juergenwt]

If you want to use two round dowel pins to locate a second part slip fit and absolute accurate you must drill and ream both parts clamped together and than hone the holes on one part to a slip fit. For a second part to fit exactly the same use the part with the pins as a drill/reaming jig. If you can not do this for some reason than one side will need a diamond pin. In that case the tolerance should be (depending on the base dim.) +/- 0.01 mm (jig bore). If you are making a production part all depends on the production method. There are many unknowns in your question.

 

[KENAT]

4. Roll pins/Spring pins instead of dowel pins - not suitable for all applications.

Also, keep the projecting dowel pins very short if possible to alleviate 'projected tolerance' issues.

Posting guidelines faq731-376

http://eng-tips.com/market.cfm?

(probably not aimed specifically at you)
What is Engineering anyway: faq1088-1484​