Tap cutting oversize! How to fix or problems to look for??

I have a problem at work and not sure what to do/how to fix. I have a 2-56 STI thread cutting tap (3B) that is cutting oversize. The NoGo gage is going in very easily, yes, it is also a 3B gage. Here is what I mean by "not knowing what to do or how to fix it" -

The drilled hole is to size, called out in a couple different charts as a 3/32". I checked the hole size, a .094 gage pin goes in, a .095 does not.
The Helicoil chart I have says the hole should check from .089-.096 after it is tapped. I check the hole at .094/.095 after it is tapped.

So all the data (although limited) says I should have a good thread, or at least everything up until the threading part is correct. What else can I do or check if my holes (before and after tapping) are within spec? To note, the thread gage (Balax brand) lists the GO as like .0963 and the NOGO as .0976 (or something close, I remember it is only .0013" difference between them). Here are the details I can think to list -

OSG brand tap, 2 flute, spiral point
Solid (not the spring loaded kind) quick change holder, runout TIR less than .002
840 rpm, 15ipm
Haas UMC-750 with rigid tapping, retract speed set to 2x
6061 aluminum plate material
Castrol Hysol MB50 (I think that is the brand, not at work now) at approx 10% mix

A few questions up front, could the gage be wrong by any chance? It is brand new with certs FYI, but mistakes happen... Could the tap be labeled wrong or be bad? Seems like .0013" total is awfully tight for a $20 tap, but I am not familiar with all the different classes of fit. If I drill the hole undersize (next drill would be .0895, I think) would it make a difference on the thread gage? Not really too familiar with thread gaging, most places I been it has always been just tap it and if the bolt threads in and gets tight its a "good" thread...
It's possible I don't have a 3B tap, not at work to double check this, but pretty sure I checked this to the print spec so I ordered the 3B gage, I assume (you know how that goes!) that I also ordered a 3B tap at the same time... To that point, anyone know the difference in spec between 2B and 3B? Is it enough that a 2B tap/thread is bad checked against a 3B gage?

Lots of ground to cover here. The actual measurement on the go no-go gages is the pitch diameter. Not the starting hole (pilot hole) diameter. Your tap is cutting oversize making your pitch diameter too big. It has very little to do with your starting hole. What I would do if this nightmare was here, is get out my pitch diameter mics and start measuring both the tap and the gage. You can measure pitch diameter using gage pins and measuring over the pins, too but you have to fumble around and get everything lined up.

If your gages are correct within reason... no gross errors and your tap is correct within reason then it is in the machining process, most likely. If your rigid tap isn't synched well it could dwell and cause oversize threads.

Before doing any of this I would hand tap a hole in scrap to make sure it isn't rigid tap dragging or pushing the tap too fast.

I know I didn't answer your whole question. You will need to study pitch diameter if you are unfamiliar with that concept.
Best of luck.
Greg

What he said -- first tap a couple holes by hand, see what you get. That should get you some info about the tap. I will point out as well that you seem to be operating right at the top of the hole tolerance, and your statement about TIR on the rigid holder ("less than .002") says to me that if you have .0015 TIR on the tap, you are maybe opening up the pitch diameter of the tapped hole by as much as .0015, assuming everything is perfectly rigid (unlikely, but a useful example). A floating tap holder might be a better choice, but I'm not a CNC expert by any means.

If that stuff doesn't help you figure it out, then start measuring the tools.

I've not seen anyone spec 3B and a helicoil at the same time. Maybe you can talk the designer into using a keysert?

Any chance you can get the TIR of the tap any better? .002 run-out and .0013 difference between a good thread and a bad thread may be your problem.

specfab said:

What he said -- first tap a couple holes by hand, see what you get. That should get you some info about the tap. I will point out as well that you seem to be operating right at the top of the hole tolerance, and your statement about TIR on the rigid holder ("less than .002") says to me that if you have .0015 TIR on the tap, you are maybe opening up the pitch diameter of the tapped hole by as much as .0015, assuming everything is perfectly rigid (unlikely, but a useful example). A floating tap holder might be a better choice, but I'm not a CNC expert by any means.

If that stuff doesn't help you figure it out, then start measuring the tools.

Click to expand...

I agree I am at the high end after the hole is tapped according to the Helicoil chart. If I had checked this before selecting the drill I might have started with the smaller drill to begin with. I just assumed if a 3/32" was called out and it cut to size I was good to go... Helicoil - http://www.helicoil.in/pdf/helicoil catalogue.pdf - actually recommends an even larger drill for harder materials, .096" (#41). This would put the hole at the very high end, are they assuming the tap will "push" some material back into the hole, or that the drill cuts perfectly to size? Just wondering if I need to double check all the drill sizes (looks like we will be doing lots of these style of parts with tiny helicoils) beforehand or if this is an anomaly....

I will try tapping a few by hand and see if its a machine problem, thanks for the tip!

GBeaman said:

Lots of ground to cover here. The actual measurement on the go no-go gages is the pitch diameter. Not the starting hole (pilot hole) diameter. Your tap is cutting oversize making your pitch diameter too big. It has very little to do with your starting hole. What I would do if this nightmare was here, is get out my pitch diameter mics and start measuring both the tap and the gage. You can measure pitch diameter using gage pins and measuring over the pins, too but you have to fumble around and get everything lined up.

If your gages are correct within reason... no gross errors and your tap is correct within reason then it is in the machining process, most likely. If your rigid tap isn't synched well it could dwell and cause oversize threads.

Before doing any of this I would hand tap a hole in scrap to make sure it isn't rigid tap dragging or pushing the tap too fast.

I know I didn't answer your whole question. You will need to study pitch diameter if you are unfamiliar with that concept.
Best of luck.
Greg

Click to expand...

What do you mean by that (I changed to bold type)? Is this a common problem, or hard to fix? FWIW I have 8 holes in each part and 55 parts to run, should I expect this to be problematic?

A couple of thoughts.....this is what I would do
#1 verify that the machine is actually programmed for rigid tapping the hole
#2 my experience says when tapping aluminum you are better off with uncoated taps....is your coated? (I do not do a lot of aluminum)
#3 some coolants just don't have the lubricity needed for aluminum....stop the machine and give it a shot of moly dee before tapping.
#4 you say runout is less than .002"....on a 2-56....that seems like a lot (% age wise)


just my random thoughts on the subject....
good luck

screensnot said:

I've not seen anyone spec 3B and a helicoil at the same time. Maybe you can talk the designer into using a keysert?

Click to expand...

Not a chance, aerospace part been in service for some time now. Not sure if the last shop made a "good" thread or not but I assume they did as we have full inspections/ppaps. I have no way to check or verify any of this, I just have the print.

bigjon61 said:

Any chance you can get the TIR of the tap any better? .002 run-out and .0013 difference between a good thread and a bad thread may be your problem.

Click to expand...

I could put the tap in a collet and get it better I suppose. I thought the tap is mostly guided by the drilled hole, would the runout actually make the tap cut bigger? I know an endmill obviously cuts bigger with runout, just thinking a tap is following a drilled hole, but of course we are talking .0013" ... I will keep this in mind.

6061Mike said:

Not a chance, aerospace part been in service for some time now. Not sure if the last shop made a "good" thread or not but I assume they did as we have full inspections/ppaps. I have no way to check or verify any of this, I just have the print.



I could put the tap in a collet and get it better I suppose. I thought the tap is mostly guided by the drilled hole, would the runout actually make the tap cut bigger? I know an endmill obviously cuts bigger with runout, just thinking a tap is following a drilled hole, but of course we are talking .0013" ... I will keep this in mind.

Click to expand...

I would try to get te tap as close to 0 runout as you can......especially in soft materials a tap can / will act like a single flute cutter.

toolsteel said:

A couple of thoughts.....this is what I would do
#1 verify that the machine is actually programmed for rigid tapping the hole
#2 my experience says when tapping aluminum you are better off with uncoated taps....is your coated? (I do not do a lot of aluminum)
#3 some coolants just don't have the lubricity needed for aluminum....stop the machine and give it a shot of moly dee before tapping.
#4 you say runout is less than .002"....on a 2-56....that seems like a lot (% age wise)


just my random thoughts on the subject....
good luck

Click to expand...

#1 yes it is rigid tapping I am positive
#2 it is coated, elektralube. curious why this would make a difference, wouldn't the coated tap have to meet the specs as well as uncoated?
#3 worth a shot, although I don't have molydee I can probably find some tapping fluid
#4 good point, already noted

thank you for taking time to help! (:

I had a plague of unbelievable coincidences a couple years back. I machined a thread undersize and bought a very expensive 2.0" Royal brand tap to chase with. The tap was undersize. Couldn't believe it. They wouldn't RMA my tap either because I had ground the leading few threads off of it. Regardless that they had manufactured the pitch diameter out of tolerance. ARRGHHH... Then soon there after I got 2 ring gages from same company that were either mislabeled or ground too small, read that 2!! One is wrong I tell the company they send a replacement the second is wrong! So I ordered a gage from Vermont after being late on parts, holding up the machine, trying like you to figure out what the crap is going on! The ring gage from Vermont was OVERSIZED!!! Certs and NIST standards in the box. My male plug gage would go into the ring gage! Aint supposed to be able to do that! Taps you assume should be right. Gages you assume should be right! Moreover gages from 2 different companies. It turned into a nightmare.

It may be very simple in your case. But surely, you planned to run out drill and tap the holes. They fit the gage... ship the parts. Now you are in for checking this that and the other until spec that should be easy to obtain is reached. Just doesn't sound like fun. The nightmare may not be one or it could be a real hairy ordeal, but it surely isn't as simple as you had planned.

When you discover and fix the problem you should get repeatable results.

How many taps have you tried? How about a form tap? They are the best for cutting to size, IMO.

GBeaman said:

.....

It may be very simple in your case. But surely, you planned to run out drill and tap the holes. They fit the gage... ship the parts. Now you are in for checking this that and the other until spec that should be easy to obtain is reached. Just doesn't sound like fun. The nightmare may not be one or it could be a real hairy ordeal, but it surely isn't as simple as you had planned.
...
.

Click to expand...

Yes, I thought I would drill and tap them and be done. I assumed (that damn word again!) I would be fighting a flatness issue (thin-ish part with lots of pockets/cutouts), and run time. Now I have to chase this crap down.
I appreciate the help and thoughts so far. I have alot of options to look into Monday!

6061Mike said:

#1 yes it is rigid tapping I am positive
#2 it is coated, elektralube. curious why this would make a difference, wouldn't the coated tap have to meet the specs as well as uncoated?
#3 worth a shot, although I don't have molydee I can probably find some tapping fluid
#4 good point, already noted

thank you for taking time to help! (:

Click to expand...

I have no experience wit Elektralube and I am not sure what it actually is............I will relay what I have been told.....with coatings like AlTin...the Al is aluminum........Aluminum works great for coatings on tools used for steel...but using a tool coating that contains aluminum to cut aluminum is a recipe for sticking and galling.

DavidScott said:

How many taps have you tried? How about a form tap? They are the best for cutting to size, IMO.

Click to expand...

This was my first 2 parts, only have one tap at the moment. I omitted form taps for STI (although in my limited experience they are pretty kickass in the right materials) because I did not have a handy chart for form tapping STI. In hindsight, looks like my "handy chart" is not so handy after all as my drill is actually to the high side..

Anyone have a form tap chart for STI, or the formula for figuring?

toolsteel said:

I have no experience wit Elektralube and I am not sure what it actually is............I will relay what I have been told.....with coatings like AlTin...the Al is aluminum........Aluminum works great for coatings on tools used for steel...but using a tool coating that contains aluminum to cut aluminum is a recipe for sticking and galling.

Click to expand...

Yes I know AL coatings are not for aluminum, I usually go ZrN or TiB2 if I can, or polished "bright" uncoated. This is from MSC website -

elektraLUBE® prevents welding, loading and galling between the tap and the workpiece. It is commonly used on stainless steels, high nickel alloys, aluminum and copper. elektraLUBE® is a proprietary coating exclusive to OSG Tap and Die, Inc.

Not trying to hi-jack the thread, but where do you find standards for STI threads? My Machinery Handbook 29th edition only has metric info.

I think Balax's web site would have the info. They are my preferred tap for any application, and only a state away when I need something that is not stocked locally. I will also vote no on coatings for precision tapping in aluminum, especially the little buggers. For what you are doing I would use a Guhring or Titex aluminum specific stub drill and a Balax form tap. Murphy's law, get extras so you don't need them.

I would float that tap!

I would not use a floating tap holder tho.

Get a floating reamer holder. This will give your tool just enough wiggle room to align with the hole and not try to influence it in any regards to TIR.

Not only that - but the floating holder will also allow a slight amount of variation in Z as well. Your troubles could be from an ever so slight Following Error in Z/S in the tiny values that you are werking with here.

An actual tap holder would prolly werk OK, but I like the reamer holders better as they don't have near the free travel that is assosiated with a tap hiolder. The free travel can at times get you in trouble by not re-seating exactly the same every time, and possibly going too deep - which prolly is not an issue in this app, or is it?

I find floaters are a completely under-appreciated tool in this forums circle. "Rigid and tune" seems to be the "right" way.
For Petey's sakes - quit the fight and float it. Save the rigid holders for spot drills and end mills...
(Makes me the back woods hack... )



Still - a Class 3 in STI just seems SO messed up...



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

Think Snow Eh!
Ox