Pipe Taps

[Brian B 74]

Looking for a chart somewhere that gives a general idea how deep to push a pipe tap reamer and a pipe tap in a NC machine. Anyone know where I can find one?

 

Thanks!

[K2csq7]

Can't help you with a chart, but I used to ream till the correct dia was reached, then tap on the machine only enough to get it started and finish by hand. Staggered tooth taps worked the best for me. From what I hear now, threadmilling them is the way to go.

HTH

[Mgrenier]

Here are the values we use for taps:

 

1/8-27NPT: .480" DEEP

1/4-28NPT: .736" DEEP

3/8-18NPT: .775" DEEP

1/2-14NPT: .965" DEEP

3/4-14NPT: .900" DEEP

1-11.5NPT: 1.150" DEEP

1-1/4-11.5NPT: 1.230" DEEP

 

We use OSG's list 12053 tap that are interrupted threads spiral fluted and they work very well.

 

We never bothered with the taper reamer...

 

HTH

[crazy^millman]

Threadmill it and done. I got away from tapping NPT on the machines years ago.

[spade117]

Definitely threadmill.

 

If you are using a tapered reamer beforehand, describe it as a tapered endmill with the proper dimensions in mastercam and works pretty well.

[Brian B 74]

Thanks for the input guys! Greatly appreciated.

[Mic6]

Last time I rigid tapped NPT...the tap went SQUEEAAAAL....POP! Threadmill please!

[CJep]

I used to rigid tap with NPT in the Bridgeport,..I'd chuck it up in a keyless, flip the switch, let the tap catch the first couple of threads, kill the power and finish it by hand. I kept a NPT plug in my tool box that I used as go/no go.

[BenK]

+1000 to threadmill

[Brian B 74]

We were having a conversation in the office today about threadmilling. We don't normally threadmill here but the block is 50+Rc and need to put a vacuum line in it. According to an article on CTE Mag's website (click here) it says it is not recommended to ream prior to tapping. I was looking on Chicago Latrobes website under their pipe reamers. It says there that the diameter of the hole at the top of a 1/8-27 after reaming and prior to tapping is .338 - a tap drill size is .332. Is it really worth reaming then?

[crazy^millman]

Threadmilled 50+ RC with no problem and the right threadmill will cut the taper and put the correct radius on the the top of the threads at the correct angle without pre-reaming the hole.

[K2csq7]

+1 more for threadmilling, Tapping em on the machine always failed unless we planned on finishing em by hand.

Do WHATEVER you can to get a sacrificial part (or at least a pc. of the same material heat treated & all) to run tests cuts on before doing it on the actual part. It will not only allow you to get everything dialed in correctly, but also give you and the operator the confidence to push the button.

[Cannon]

Im going to threadmill a pipe thread next week and need some advice. So I just drill it to smaller thread hole diameter, feed threadmill to final depth and cut from there?

[xycnc]

Carmex has tapered endmills at the 1.47 deg so if you dont want to run a reamer in them you can circle mill it helps to improve thread mill life. I use as a starting point the effective thread Length as my depth from my Handbook and then the Outside dia for my major thread dia. Then once you get it programed save it and you just import it in when you need it again.

[Thoob]

I use 2d contour in my mill with a bullmill. The contour is drawn what the top of the taper diameter is. I use a .03 rad insert. In the depth parameters I select .01 max rough step, select keep tool down and check tapered walls, then put in the taper of the pipe thread hole. (1.783) It gives me a nice tapered hole and my threadmills run perfectly.

[Brian B 74]

Do you guys thread mill from the top down? Or bottom up? And if your mill has multiple teeth do you do one pass?

[mold100]

Bottom up always, using active nuber of teeth buried in hole, never single pass I usually use 3 multi passes 1/4 and above, 4 or 5 if down to 6-32. If you thread mill pipe threads be sure to add taper of 1.78333 typical for 1/8 npt threads.

[Brian B 74]

Thanks for the info. Will give it a try.

[Diesel Tom]

+1 thread mill all pipe taps and you will never look back they last a long time I just did a 16 core and cavity total of 64 all taped with same thread mill and it still look s like new

[Brian B 74]

My issue in the past with thread mills was they would chip the tip after about 6-8 holes. So I haven't used them much.

[Brian B 74]

Today I received my indexable Carmex thread mills (14 and 18 NPT). For those of you who use them - is there a general rule of thumb as to your final depth? Do you go the full length of the tool holder (L1 dim)? Do you go the normal depth of the pipe tap?

[Tim Johnson]

I go by Machinist's Bible L1+L3 on depth & E3+h on diameter. I don't get any complaints.

[Brian B 74]

Thanks Tim. I will give that a try.