What's new
What's new

Rigid Tapping Accuracy

MRudisill

Plastic
Joined
Jan 13, 2020
Hey guys,

Wondering if anyone has experience rigid tapping very fine threads like 2-56 with a standard rigid tap. I have cut down to 6-32 and obviously rigid tapping works great overall, but is it accurate enough to get proper threads on something as small as 2-56? Someone has mentioned using a tapmatic holder, but for the times here and there we do some 2-56 I dont think it would be worth blowing a few hundred bucks on a holder (yet).

Using a brand new Haas SMM2.
 
We rigid form tap 0-80 all the time. BUT it's all for our own product line so we aren't gaging to a 2b or 3b spec...
 
Just had a suggestion for form tapping since I mainly cut aluminum. Any suggestions on that? Do you guys use standard taps, forming taps? Haven't done much tapping on the machine so just trying to get as much input as I can and get a good system in place.
 
I've form tapped lots of small threads in Al -- M2.0, 2-56, etc. They have always gaged fine. Just have to be very careful with the drilled hole size, since with small threads, just a thousandth off on the hole size can play hell with form taps.

Regards.

Mike
 
Noted, thank you. Just got a brand new master drill set so I will make sure to get it exact. Glad you said that because I am used to a thou or two being no big deal and just getting a close drill size.
 
I have also tapped many many holes at 0-80 and 2-something in Stainless Steel. The machine holds the tap straight and true, much easier than a human.

I recommend everyone check the tapping tables in your Machinery's hand book. Depending on how deep you are tapping, the size of the acceptable hole changes a lot. For example, if you are doing a 1/4-20 hole about .25 deep, you are fine with what most tapping charts give for the drill (which is .201"). But if you are going 3/4 of an inch or so that hole size jumps way up to about .207."

And, this still maintains spec for the thread type.

Mike
 
1) tapping rpm might be limited. at higher rpm some machines have more trouble stopping spindle, as long as spindle rotation slowing and Z axis move in sync usually it works. if spindle still turning and Z not moving tap tries to pull out of holder. it using setscrew it usually slips. collet might hold so good to not allow tap to pull out
.
2) extension compression holders are common and would help if having problems. I often see tap screw in extra cause spindle not stopping fast enough. when tap pulls out of hole usually see tap spring back once free of hole
.
I have seen rigid tapping where Z travel soft limit tripped and machine stops spindle and Z travel and
even a M5 tap doesnt break from sudden stop. of course spindle rotation to Z travel might be .0002" or more in error. in that case setscrew holder easier to loose setscrew and handle mode tool holder off the tap stuck in the hole
 
I have also tapped many many holes at 0-80 and 2-something in Stainless Steel. The machine holds the tap straight and true, much easier than a human.

I recommend everyone check the tapping tables in your Machinery's hand book. Depending on how deep you are tapping, the size of the acceptable hole changes a lot. For example, if you are doing a 1/4-20 hole about .25 deep, you are fine with what most tapping charts give for the drill (which is .201"). But if you are going 3/4 of an inch or so that hole size jumps way up to about .207."

And, this still maintains spec for the thread type.

Mike
.
drilled hole size is not always size of drill bit. I have seen damaged or poorly sharpened drill bits drill way oversize holes before, .040" bigger than drill bit not unusual. of course normally drilled hole is within .005" of drill bit size, just saying not always
 
Just had a suggestion for form tapping since I mainly cut aluminum. Any suggestions on that? Do you guys use standard taps, forming taps? Haven't done much tapping on the machine so just trying to get as much input as I can and get a good system in place.

Definitely go with a form tap for aluminum!! We use everything from accupro brand to balax. Modified bottoming thread. With a standard 118deg drill point you can tap a 0-80 to .020" shorter than drill depth, 2-56 .025" shorter, and 4-40 .030" shorter.
 
Hey guys,

Wondering if anyone has experience rigid tapping very fine threads like 2-56 with a standard rigid tap. I have cut down to 6-32 and obviously rigid tapping works great overall, but is it accurate enough to get proper threads on something as small as 2-56? Someone has mentioned using a tapmatic holder, but for the times here and there we do some 2-56 I dont think it would be worth blowing a few hundred bucks on a holder (yet).

Using a brand new Haas SMM2.

Noted, thank you. Just got a brand new master drill set so I will make sure to get it exact. Glad you said that because I am used to a thou or two being no big deal and just getting a close drill size.
The term Master drill set kinda scares me....

make sure you look up your minor dias for a 2-56 in the spec you need to use, Ie 2b 3b
for a 2b its .0772 to .0744 minor dia. use the biggest drill you can on the minor with out going over. sometimes you have to go metric.
make sure you chekc the minor with a pin also as a not straight hole will break taps.
we do lots of 0-80, 2-56 cut taps and dont have problems rigid tapping.
 
The term Master drill set kinda scares me....

make sure you look up your minor dias for a 2-56 in the spec you need to use, Ie 2b 3b
for a 2b its .0772 to .0744 minor dia. use the biggest drill you can on the minor with out going over. sometimes you have to go metric.
make sure you chekc the minor with a pin also as a not straight hole will break taps.
we do lots of 0-80, 2-56 cut taps and dont have problems rigid tapping.


Lol master set as in a full english, metric, lettered set that is only to be used on the CNC.Not beaten the hell out of in a dewalt somewhere else in the shop then trying to precision machine with it lol. And I will keep those other notes in mind.
 
The old charts that people still use is based on the outcome of using those old drills that produced the oversized holes. Unless yuo are using defective drills, holes are rarely out more than a thousandth or so these days with a good brand drill.

If you are a modern machine shop, you should be using 135 deg split point drills whenever possible. I almost never use 118 deg drills, as they tend to "walk" and that will cause hole inaccuracy.

Invest in one good combo set, drill index, (letter, number and fractional) set of 135 deg split point short drills (usually called machine screw drills}. The are shorter, more straight and rigid and produce the most accurate hole sizes. Note: a good set is about $500.00, but after that just order single drill to use as replacements.

Never use, "damaged or poorly sharpened drill bits."

Mike
 
Just did a bunch of 000-120 in the TM1. Easy. Form Balax Tap so heads up Mike, the form tap drill size is .031. After tapping the first one just shy of the depth, I form tapped it a bit more with another tap and it has very little torque resistance. Material is 7075 T6, 1000 RPM. I'm not sure if there is a cut tap for this size except maybe in watchmaking.
 

Attachments

  • Laser Tapping.jpg
    Laser Tapping.jpg
    90.7 KB · Views: 43








 
Back
Top