Hole diameter for screws

[davidrdguez]

Hi everybody!

I'm designing some unions with screws. Let's say I have to put together two sheets. The screw goes from the top and the lower sheet has the thread.

If I'm using e.g. an M5 screw; what should be the diameter of the hole of the top sheet? 5 mm?? a bit more?

I got some accurate rails. The holes in them are 4,5 mm. This allows certain game for precise positioning. I'm confused

Attached a picture

Thank you!

http://files.engineering.com/getfil...12de-4353-bdb2-e162cebb7022&file=diameter.jpg

 

[drawoh]

davidrdguez,

You need to read up on GD&T, and work out tolerances. Let's plug in some numbers.

Your lower piece has M5X0.8 tapped holes, located to a positional tolerance of 0.2mmDIA. You can read up on projected tolerance zones, or add 0.1mm for good luck. This should account for your tapped hole not quite being perpendicular.

Your minimum clearance hole diameter at perfect position is 5mm + 0.2mm + 0.1mm = 5.3mm. Add your positional tolerance to this, to get a clearance hole guaranteed to work. If your clearance hole is positioned to 0.2mmDIA, your clearance hole must be 5.5mmDIA.

This all is fairly simple geometry.

JHG

 

[KENAT]

Check out appendix B of ASME Y14.5M-1994 or similar it shows you the equations to use. I've even posted about it over in GD&T before with a spreadsheet and examples.

You have to allow clearance that accounts for the locational tolerance of not just the through holes but also the locational tolerance of the tapped holes & of course the size tolerance of the through holes themselves.

Per ASME Y14.5M-1994 (slightly clarified) lets say:

H = F + T(thread) + T(clearance)

Where:

H = Minimum diameter of clearance hole (MMC limit)

F = Maximum diameter of fastener (MMC limit)

T(thread) = Positional Tolerance Diameter for threaded holes

T(clearance) = Positional Tolerance Diameter for clearance holes

MMC = Maximim Material Condition (ie. smallest hole, largest shaft etc.)

Now, often times folks make T(thread)=T(clearance) but given that threaded holes have an extra process step adding to the tolerance, & they don't really benefit from 'bonus tolerance' (yes Mike I said it) then for anything approaching tight tolerances I tend to favor the threaded hole slightly so maybe split the toll ratio of 3:2 in favor of the threaded hole. Or even better, base it on your actual process capability.

3*T(clearance) = 2*T(thread)

This assumes you're using positional tolerance (part of GD&T which was developed exactly because of this kind of situation - getting patterns of holes to match up without making tolerances unnecessarily tight).

Posting guidelines faq731-376

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

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

 

[KENAT]

Forgot to say, the above assumes thin plate and/or that you add projected tols separately.

And by the way, in your sketch, the head of the screw appears sunk into the hole or am I mistaken?

Posting guidelines faq731-376

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

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

 

[ShaggyPE]

Here is a calculator utility for your application:

http://www.engineersedge.com/fixed_fastener.htm

-Dustin
Professional Engineer
Pretty good with SolidWorks