threads

[fourperf]

hi guys, I posted this in the general forum but got no response so I thought I would try here (many very helpful here). What is the best/easiest way to figure out major/minor diameter for non-standard threads. for instance a
2.75 -12tpi threaded boss. The od/major dia would be 2.75 how would I figure out the minor dia and the same goes for the female threaded piece. I find the machinists handbook overwhelming and was wondering if there was a relatively simple formula.

thanks

mark

[extanker59]

It is in the book. Well, a 2.75-12 UN thread is in the book. Is this thread form the one you want? OD is 2.7481-2.7367 for the 2A class. Just start using the book and it'll get easier.

[Geof]

The 'simple formula' I use for non-standard threads is to use tap drill sizes.

The tap drill for 9/16"-12 is 31/64" for a 75% thread.

The difference between 9/16" (0.5625") and 31/64" (0.4344") is 0.1281" but because this is for a 75% thread the double thread depth is about 0.170", half the thread depth is about 0.085". Remember the 0.170" is a diameter measure; I have occasionally forgotten that then wondered why things came out looking funny.

If I was making a 2.75"-12 thread I would first make a set of gauges.

The OD of a thread is slightly smaller than the nominal size and if you want to dig into Machinery's Handbook (which I do not ) you can find the exact formula, I use 5% of the double thread depth which is 0.05 x 0.170" = 0.008", so I would turn the stock to 2.742" +0.000" -0.002".

Using a full from threading tool the full depth of cut is the true thread depth but because my sizes are estimates just sticking these into a threading command could result in the tool cutting too deep so I always go shallow on the first run through. On a lathe I use G92 so I can control the final depth quite easily; on the mill I simply put something like (+)0.010 in the wear because I always use tool comp for thread milling.

The way I check for the correct threading depth is by feel or with a powerful magnifying glass. When a full form threading tool is exactly at the correct depth the crest of the thread is blended into a nice radius and this can be felt and seen quite easily. Actually if you cover the part with felt pen ink you can see quite easily how close you are to full depth during the first run through. Normally what I do is stop just a trace shy of completing the crest radius, leaving just a trace of a flat top.

For the female gauge the nominal size of the hole is 2.750" -0.170" = 2.580" but I would bore it 0.020" oversize, possibly a little more because an 80 to 90% thread is more than adequate for anything. Then I would adjust my initial threading depth to allow for this on the first run through and then tweak the wear or G92 X values until I had the fit that I wanted.

If I am getting really carried away about getting my production threads between repeatable limits I will make Go and No-Go for both male and female but most times I do things by feel.

If I am getting really picky I will measure the final threads with a micrometer and the little wedge block things I have that always fall on the floor when I am doing this; normally I just keep the gauges in case replacement parts have to be made in the future.

[fourperf]

Hey Geoff, thanks for the explanation. I dont get the double thread depth part

but because this is for a 75% thread the double thread depth is about 0.170"

how did you get from .1281 to the .17?

thanks a lot

Mark

[Geof]

Originally Posted by fourperf .......how did you get from .1281 to the .17? thanks a lot Mark

0.1281 divided by 0.75 equals 0.170

[fourperf]

got it.

thanks a lot

mark

[ken70ss396@yaho]

Use the machinist handbook religiously. And get a set of thread wires. Learn to use the 3 wire set with micrometers and you'll be producing perfect threads.If you have a large production run of parts a thread ring gage is worth the expense.