How to spec position of Shoulder Bolt holes?

[thebuc1010]

Hey all.
I've been put to the task of drafting up drawings of a ~15 part precision optic system. Fortunately I've personally already made all the parts on the CNC, and I know that a large scale production shop shouldn't have a problem producing the pieces.
Many of the pieces are attached/aligned together with shoulder bolts.
example: for use with two 4-40UNC-2a,0.125shoulder bolts
piece 1 has a countersink and a 0.125reamed through hole
piece 2 has a 0.125reamed ~.1 deep hole with 4-40UNC-2B concentric tapped threads.

how the heck should i spec this out in a reasonable manner? it seems to me that putting the tight position/size tolerance i need to get the shoulders to line up usefully forces the 4-40thread location to have an excessively small position tolerance.
Machineries handbook says 4-40 2a screws have an allowance of 0.0008. How do I use this information effectively?
Perhaps I'm over thinking this.

Attached is my thought on how to do it with part#2. I was going to put the same position/size tolerance on part #1's reamed section. Does it make sense?

 

[KENAT]

I think you may be a bit mixed up, plus some of those tolerances end up looking pretty tight.

Maybe take a look in ASME Y14.5 (I'm assuming 94 edition) Appendix B for how to calculate tolerances for making hole patterns etc.

Posting guidelines faq731-376

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

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

 

[powerhound]

Yes, it makes sense to use positional tolerance anytime you are trying to locate a feature. That's the only way it's supported in the standard. A few points on your current print.
1. Using the diameter symbol on a flatness callout is incorrect.
2. You need datum references in the feature control frames that control the 4-40 holes.
3. You should not specify a ream. Simply give the size and let the shop provide the part.

Other than that, it looks good. I'm glad to see a good use of the projected modifier.

Powerhound, GDTP S-0731
Engineering Technician
Inventor 2013
Mastercam X6
Smartcam 11.1
SSG, U.S. Army
Taji, Iraq OIF II

 

[thebuc1010]

Thanks for reply kenat.
I have the 1982 y14.5 in my possession and 2 books on GD&T. I've read the section on positioning extensively. And i've downloaded your spreadsheet on fixed fasteners.
All that matters in this part is that one lens, the one in the 45degree plane, gets placed well relative to these shoulder bolts. The position of the walls relative to these holes is nearly irrelevant.

Also the tolerances are tight. They need to be right? or what else is the point of having a precision shoulder bolt in an un-precise hole? The part is only about 1 inch^3 so in my mind it shouldn't be incredibly difficult to hold good tolerances over such small distances.

 

[thebuc1010]

Thanks powerhound.
1) oops yeah i haven't double checked everything like that yet. Definitely going to fix them up before i finalize this drawing.
2) Indeed. I've been wondering how to do it actually. I'm not interested in the holes position relative to any side walls. So is it okay to just put only reference datum B?
3)Okay. I was following a tip I had read in another book written by an expert machinist who sometimes thought it was convenient to have a hole specified as reamed or drilled so he doesn't waste his time beating his head over what an engineer was originally thinking. I personally thought reaming the holes was essential when I CNC'd the parts. Though I do agree I'd prefer to be more ambiguous in a drawing so a manufacturer can decide what is best.

 

[KENAT]

Sounds like you have more machining experience than me but I typically shy away from very tight position tolerances on threaded holes as they can be tricky to manufacture to. In that case I'd tend to have separate dowel pins for alignment or similar.

However, I don't have the information on your assembly etc. so am not sure what the screws are actually doing.

My spreadsheet should help, make sure you have the latest version and look at the examples on the later tabs.

Posting guidelines faq731-376

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

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

 

[thebuc1010]

Kenat, Your spreadsheet and examples have been extremely helpful.

Yes I agree after learning a lot about GD&T and personally struggling with spec'ing these shoulder bolts I would much rather prefer to have alignment dowels and then just clearance screws to tie the pieces together on the side.
But it adds more pieces into the assembly, the dowels. Shoulder screws are basically precision dowels and a screw in one piece. And I don't think I can make that drastic of a change in the design at this point, especially if its just to make my life easier when I make the drawing specifications.

Has anyone successfully worked with and made a good drawing for shoulder screws before?
Maybe you are right and they have just been a terrible idea from the start.

 

[SeasonLee]

Fundamental Rules (e) on ‘09 standard page 8 says:
The drawing should define a part without specifying manufacturing methods. Thus, only the diameter of a hole is given without indicating whether it is to be drilled, reamed, punched, or made by any other operation….

SeasonLee

 

[KENAT]

It's really not just the drawing, it's the functionality, the manufacturability...

Sure I've used precision shoulder screws before. However not for typical hole pattern situations. If I was using them I'd probably go with one mating hole and one mating slot assuming this functionally worked (for more than 2 screws I'd probably make the other holes more generous clearance).

If you're happy that you, and any competent machine shop, can get .002 positional tolerance on those threads then more power to you. Best I've ever got a machine shop to agree to was .003 and neither I or the shop were happy (but it was rescuing someone elses' design).

When you're doing the clearance calcs for a shoulder screw you have to use the shoulder max diameter NOT the thread nominal diameter (you may well have done this, I don't know).

Posting guidelines faq731-376

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

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

 

[thebuc1010]

Kenat,
My confidence on being able to get the .002 tolerance goes back and forth. At my shop we very commonly tap #2 screws (0.086 max size, not nominal) and always drill 0.089 clearance holes for them. I've never had screws not successfully mate with these parameters.
I was very surprised when I recently calculated the implied tolerance I was making the holes to. Evenly split that is .0015 on the tapped hole and .0015 on the clearance hole (unless the drill drilled a hole slightly larger.. but still a minor difference in tolerance).
So in my mind its possible.
But then I imagine some one inspecting a part and I get worried that these constraints are too high. I've never used an inspection machine or any inspection method/datum simulator to check positions. I've always just checked if the part fit into the opposing part. (well i guess that sort of is an inspection method/datum simulator in itself)

 

[KENAT]

You're probably reaping the benefits of most parts being nearer nominal etc. Plus on this kind of scale various of the parts will deform a little, or chew material off the clearance hole... and you at least appear to get away with it. Unfortunately if it's a part that is actually loaded it can come back to bite you when screw heads start popping off in service etc. (failure mode of flat head screws).

The simplistic 'worst case' type tolerancing that classic positional tolerances is calculated on is fairly conservative - some would argue too conservative.

We used to have lots of parts toleranced similar to you say, made mostly by the same high precision machine shop. Then we started sending some parts to other folk and the fit issues began.

Posting guidelines faq731-376

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

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

 

[thebuc1010]

Interesting.
Maybe I should mention these parts are made out of aluminium so it is very possible that the steel screws chew through the material and accommodate other errors in manufacturing.
And this might not even be a huge problem, these parts aren't loaded in any sense.

 

[thebuc1010]

Also,

I've been looking more at screws and thread specs for 4-40UNC-2a/2b in machinerys handbook trying to get some insight on this.

Max pitch diamater of screw 2a=.095
Min pitch diameter of internal 2b=.0958
Min clearance--------->.0008 (this is what i designed for)

Min pitch diameter of screw 2a=.0925
Max pitch diameter of internal 2b=.0991
Max clearance--------->.0066 (way more accommodating, what i wish i could design for)

Do you guys think I should still design for the worst case situation? When the range of possibilities is from .0008-.0066.
Maybe by using spec'ing .0008 a machinist knows to use a tap that will make the threads closer to .0991 to create more slop in the system but still have class 2b.

 

[KENAT]

thebuc, typically when doing these types of calcs you pretty much ignore slop in the screws. For a conventional screw you'd just use the max major diameter - which I think my examples in the spreadsheet show.

However, in your case you'd actually use the max diameter of the shoulder (plain shank).

So, Minimum mating hole diameter - maximum shoulder diameter = total positioning budget.

You then need to divide this positioning budget between the threaded holes and the mating clearance holes.

However, this assumes that the shoulder screws are being used to mount a mating part with a simple hole pattern - I'm not sure this is the case from the info you've given.

Posting guidelines faq731-376

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

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