Threading Depth 1

[mrmitche]

I am creating drawings from parts imported into Solidworks that lost threaded features. Is there a rule of thumb for how much of the hole to leave unthreaded or how far to tap past the end of the bolt?

For example, a 40 mm M8 socket head cap screw is holding two blocks together. The block the bolt passes through is 28 mm, leaving 12 mm of the screw to engage in the next block. The hole in this block is 19 mm deep. For these types of situations I've just been picking a random value greater than the screw engagement (12 mm) and less than the hole depth (19 mm), for this one I chose 15 mm. It shouldn't really affect the parts, but I was just curious if there is some rule that is generally followed like tap 2 mm past the end of the screw or leave 2 mm of the hole untapped.

Follow @mrmitche_ on Twitter!

 

[dgallup]

I usually just specify a minimum full thread depth that is deep enough that the end of the bolt will never bottom out. For that you need to know the length tolerance on your bolt and the thickness tolerance for the block you are going through. That gives the machinist the most tolerance.

----------------------------------------

The Help for this program was created in Windows Help format, which depends on a feature that isn't included in this version of Windows.

 

[KENAT]

Typically it's good to allow for <at least> (edit) 3-4 thread pitches past the end of the screw to allow for tapping without needing a bottom tap.

However, you don't need to explicitly specify that on the drawing per any drawing standard I'm familiar with - though I'll often model it in the 3D to see if I'm causing issues.

On the drawing I usually spec things like this unless there is some other functional constraint:

"<MAXIMUM CALCULATED SCREW ENGAGEMENT INCLUDING ALL TOLERANCES> MIN FULL THREAD DO NOT BREAK THRU"

e.g in your case might be something like "12.5 MIN FULL THREAD DO NOT BREAK THRU"

Posting guidelines faq731-376

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

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

 

[mrmitche]

That makes way more sense, thanks for the information guys.

Follow @mrmitche_ on Twitter!

 

[juergenwt]

There is no standard for drilled depth of tap holes. Best is a thru hole. A lot depends on the length of the screw and how much of it is engaged. 3-4 threads is most likely a little short. I usually add the nominal thread size i.e. M6 drill 6mm past the tapped depth. Don't forget you need room for chips because most taps will push the chips to the bottom. So many variables.

 

[TWJR]

There is no standard for drilled depth of tap holes. Best is a thru hole. A lot depends on the length of the screw and how much of it is engaged. 3-4 threads is most likely a little short. I usually add the nominal thread size i.e. M6 drill 6mm past the tapped depth. Don't forget you need room for chips because most taps will push the chips to the bottom. So many variables.

The bottom line is, there is no "rule" that will fit all cases. Common sense coupled with some machining knowledge is what's needed here. Ask a trusted guy in the shop, if you can. As a guy who started in manufacturing, and still programs the CNC machines here, I can't tell you how many drawings I've seen that have 3 place dimensions for tap depth (+/-.005), and/or tap depth very close to the drilled depth (no clearance for chips). As stated, through is best if you can live with it. A "much" deeper drilled hole than tapped depth if through isn't acceptable. "MIN" tapped depth is best, with "no breakout" if that is problem.
Also can't tell you how many times I've seen a part tapped deeper than the drawing states (but not breaking out), and the inspector wanting to reject the part. How insane is that?

 

[ctopher]

I never callout drill size or depth, and the thd depth is usually max or a loose tol.
Minimum 4 thds is good to use, but I will go deeper if possible. You never know which type of tap a machinist will use.
I make them thru the part as much as possible.

Chris, CSWA
SolidWorks '15
ctophers home
SolidWorks Legion

 

[JNieman]

Also, don't be the guy who calls out +/- .005 on the pilot drill diameter for a tapped hole. I had an inspector ask me how he was supposed to inspect the drill diameter on a fully tapped thru hole and wanted to reject them.
Also, don't be the guy who calls out the pilot drill diameter from the standard tap/drill chart for a hole intended for a keensert.

_________________________________________
NX8.0, Solidworks 2014, AutoCAD, Enovia V5

 

[3DDave]

There is a minor diameter listed for most straight threads, which is usually controlled by the tap drill, so there is that. One should spec the minor diameter unless it really doesn't matter. A larger minor is easier to tap but gives up a bit of strength. I think some threads are listed with 3 standard tap drills depending on the desired percentage of thread form.

I did see someone break off a couple of taps before noticing the "HT" after the tap size. They would have broken more, but ran out. Actually they didn't notice the "HT," it was just the tap was so oversized for the nominal thread size it was a quick search to determine why.

 

[dtmbiz]

General rule of thumb for a few companies that I have worked for is; standard tap drill depth = 1 and 1/2 times the thread size beyond the thread depth.

The less depth of part there is for the thread, the more consideration to the tap drill depth.