Tapping a hole twice with slightly different start heights, anyone done this?

dandrummerman21 · Nov 25, 2015

I've got some 4140 parts which get hardened to about 40-45rc, that have a 1/4-28 hole 1.5" deep. Using an OSG 1605014286 gh6 form tap with coolant thru. Excellent tap life, and the gage goes easy with a little play before ht.

But unfortunately, our first batch of parts (1000 out of 4000 total that we will run) do not gage. I ran the form tap through some of these parts, it definitely moved, it isn't just the first few threads like I hoped.

So now I'm faced with retapping all 1000 of these parts, which isn't the end of the world. But I need to figure out how to make the rest of the parts tap a little oversize.

So firstly, I'd love to find another thru coolant form tap bigger than a gh6 that I can get to reach 1.5" deep, Does anyone know of any? (I had to grind the OSG tap back a bit for that). But I've got 4 of these taps (60$ each) and I'd like to try to change the start location in Z a few tenths and run the tap cycle again.

So the real question is, has anyone done that with a form tap? Would it work? Can I move it .0005"? .0003"?? Would I be better served putting a long cut tap in a floating holder and retapping it with another tap with a bigger H?

Rstewart · Nov 25, 2015

They make +.005" over taps for material to be heat treated.

Mtndew · Nov 25, 2015

dandrummerman21 said:
So the real question is, has anyone done that with a form tap? Would it work? Can I move it .0005"? .0003"?? Would I be better served putting a long cut tap in a floating holder and retapping it with another tap with a bigger H?

Don't do it. You'll create more problems than you have.
As said above, get an oversize tap, either a +.003 or a +.005

dandrummerman21 · Nov 25, 2015

OSG has an h11 1/4-28 tap but it is not thru spindle coolant. Will probably try that. I don't think I need tsc.

If I understand right, an h11 tap is .0025 bigger than an h6, right?

BTW, I did try a cycle with moving the start point .0005 but there was no noticeable difference in the fit of the gage. I don't think I'll fool around with that any longer.

Mtndew · Nov 25, 2015

dandrummerman21 said:
OSG has an h11 1/4-28 tap but it is not thru spindle coolant. Will probably try that. I don't think I need tsc.

If I understand right, an h11 tap is .0025 bigger than an h6, right?

BTW, I did try a cycle with moving the start point .0005 but there was no noticeable difference in the fit of the gage. I don't think I'll fool around with that any longer.

A GH11 is a +.005 oversize tap.

Perry Harrington · Nov 25, 2015

Each H is 0.0005 oversize IIRC, so H6 is 6*5 == 0.003 and H11 is 0.0055 oversize.

fmari --MariTool- · Nov 25, 2015

I've done it all the time. Why not. It effectively makes the "v"s further apart which increases the pitch diameter. Major diameter and minor diameter are not changed. Nothing wrong with it other than increasing your cycle time.

dandrummerman21 · Nov 25, 2015

fmari --MariTool- said:
I've done it all the time. Why not. It effectively makes the "v"s further apart which increases the pitch diameter. Major diameter and minor diameter are not changed. Nothing wrong with it other than increasing your cycle time.

Have you done it with a form tap? I'd imagine I'd have seen a big difference if I had a cut tap, but moving .0005" seemed to do nothing. Should I have tried .001"?

Anyway, thanks for the advice fellas, I've got an h11 tap on the way, although its not thru spindle coolant, i think I'll get away with it, its just 4140.

Milland · Nov 25, 2015

If the metal's moving around on you so much that the thread's no longer right, what about the rest of the tolerances? It might be worthwhile for you to work with the heat treater to come up with another HT method that gets the material properties you need but doesn't cause as much movement.

BTW, the surface hardening that occurs with form tapping, and surface contact area of the tap thread faces makes it unlikely you can "shift" the thread like you proposed. Your test may have just moved the tap in the holder a bit. With a cut tap, yeah, it could work but is not ideal.

Oldwrench · Nov 25, 2015

If you're going to harden the parts it makes no sense to form-tap, as the properties gained by cold-working the thread are completely lost once it reaches critical temp. I would suspect the compression stress put into the walls by your forming operation is being liberated, whence the shrinkage. Try machining the threads with a sharp tap, I bet that will fix it. We get our parts hardened to around 50-53Rc and they have 5/16-24 and 10-32 holes, both machined with ordinary H3 taps. Been working fine for many years.

dandrummerman21 · Nov 27, 2015

Oldwrench said:
If you're going to harden the parts it makes no sense to form-tap, as the properties gained by cold-working the thread are completely lost once it reaches critical temp. I would suspect the compression stress put into the walls by your forming operation is being liberated, whence the shrinkage. Try machining the threads with a sharp tap, I bet that will fix it. We get our parts hardened to around 50-53Rc and they have 5/16-24 and 10-32 holes, both machined with ordinary H3 taps. Been working fine for many years.

Understood about the thread strength and stress, but I'm not doing it for strength requirements, I'm doing it to eliminate chip issues. The hole is 1.5" deep. Spiral flute taps give them long chips which sometimes don't leave the tool, even with high pressure coolant thru the collet. Haven't tried a thru spindle spiral flute tap though.

Trying an h11 form tap currently, will be sending out a partial to HT to see if the threads gage afterward.

If it matters, the material is about 1" square coldrolled, and I'm tapping in the end of the part where the saw cut was. So stresses already in the part are probably also working against me.

triumph406 · Nov 27, 2015

dandrummerman21 said:
Would I be better served putting a long cut tap in a floating holder and retapping it with another tap with a bigger H?

That's what I would do, simplest way and fastest way to fix the problem

dksoba · Nov 27, 2015

dandrummerman21 said:
If it matters, the material is about 1" square coldrolled, and I'm tapping in the end of the part where the saw cut was. So stresses already in the part are probably also working against me.

I don't have much experience here, but I'd imagine that relieving the stresses prior to machining would help.

Matt

SND · Nov 27, 2015

You mentioned the gauge doesn't go in, but do the screws that will be used with it go in fine? Odds are they fit "just right".

dandrummerman21 · Nov 28, 2015

SND said:
You mentioned the gauge doesn't go in, but do the screws that will be used with it go in fine? Odds are they fit "just right".

They do, but tell that to the Government inspector...

They get plated too. Not terribly thick, a couple tenths afaik.

Dave K · Nov 28, 2015

fmari --MariTool- said:
I've done it all the time. Why not. It effectively makes the "v"s further apart which increases the pitch diameter. Major diameter and minor diameter are not changed. Nothing wrong with it other than increasing your cycle time.

Don't know for sure, but that don't seem right to me. When you do that, you're effectively making the "V" between each thread wider, but still no bigger in pitch diameter. If the material is shrinking on him, he doesn't need wider "Vees", he needs larger diameter pitch. When you do what you're stating to do, the pitch diameter still shrinks to undersize because of the material shrinking, but gage still goes because of elongated distance between threads. I'm just thinking out loud here, but that seems very improper.

metlmunchr · Nov 28, 2015

A wider V is the definition of a larger pitch diameter.

Dave K · Nov 28, 2015

metlmunchr said:
A wider V is the definition of a larger pitch diameter.

No, pitch diameter has to do with diameter, but what's being proposed here is making it larger longitudinally. In other words, recutting at a different starting point, is stretching out that thread, rather than changing the diameter.

metlmunchr · Nov 28, 2015

Might not change the major or minor diameters, but it sure enough changes the pitch diameter.

Dave K · Nov 29, 2015

metlmunchr said:
Might not change the major or minor diameters, but it sure enough changes the pitch diameter.

I guess I'll have to agree with that, but it's changing it in a completely wrong way. As you mentioned, the major and minor do not change at all, just the distance between threads, which effectively causes the pitch diameter to change. What else is happening, is you're changing the flat that exists between threads at the major diameter. To me this seems like a "hack" way of producing threads.

Tapping a hole twice with slightly different start heights, anyone done this?

Stainless

Stainless

Diamond

Stainless

Diamond

Titanium

Titanium

Stainless

Diamond

Titanium

Stainless

Diamond

Hot Rolled

Diamond

Stainless

Diamond

Diamond

Diamond

Diamond

Diamond

Similar threads