What's new
What's new

Tapping help!

One other thing...
This shouldn't be all that relevant in this particular situation, in aluminium at that, but especially in the smaller sizes if you drill towards the maximum allowable minor diameter, you can tremendously reduce the load on taps and reduce failure rates. Drill charts tell you what size to use, but consult Machinery's Handbook for the upper limits of minor diameter. You will be doing yourself a favor. Letter and number size drills are readily available and inexpensive. This will help your expensive tap live a long and happy life while paying for itself many times over a cheap tap.
 
Stop trying to get it done with cutting taps and get yourself a quality roll form tap! That's a HAND tap and there's no chip control. That's why it's breaking.

Just be aware that hole size is larger for those and size control is critical to get the percentage of full thread form that's required.

Thanks. I got 0.287402 or 7.3mm for a drill size with the 5/16-18 roll form tap.
 
Tapped a lot of holes and some machines use pitch length regardless of of RPM. Some machines use pitch length X RPM = Feed rate. I do know that on most all machines G84 is not rigid tapping. G84.2 is the usual G code. Not sure on a Haas. Also a 5/16-18 is a little corse for a form tap but at a higher RPM would work best. Please use a Spiral flutted semi-bottoming tap at lease. I would push the tap RPM to at least 1100-1600 for aluminum. 6061 T6 I assume. Perhaps a little slower for 7075.
 
Use the Haas help page and look up the G codes. I know Haas is good about on screen help. I last programed and ran a VF-1 with a 3 digit serial number, but I remember the on screen help was great. I was just learning CNC back then.
 
A little tip to avoid your initial feed problem. KEEP IT SIMPLE. 18 pitch, 18rpms=1ipm. 180rpm=10ipm. 360rpm=20 ipm. 720 rpm= 40ipm.

I don't care what the optimum RPM is, you can always find something close that is easily divisible, makes double checking your code really easy,
and avoids mistakes, I make enough mistakes, anything I can do to eliminate them, I do.
 
A little tip to avoid your initial feed problem. KEEP IT SIMPLE. 18 pitch, 18rpms=1ipm. 180rpm=10ipm. 360rpm=20 ipm. 720 rpm= 40ipm.

Couple of years ago was tapping a bunch of 1/2-20 holes on a VMC and decided it was running fine but could stand a little more RPM. Upped the speed a few hundred in the CAM and let it rip. Unloaded the fixture to find all the holes over sized now but with out threads.

Note to self...remember mills are IPM, lathes are IPR and it does matter:(







KISS, got to love it.
 
Thread forning question

We did some of this on a difficult material,. A-286 for what it's worth. We saw that with the recommended hole size before forming the thread, we got incomplete thread crests. there was like a groove along the crest where the forming tool did not fully deform the material into full and correct thread form. From a functionality and strength standpoint I think that the irregularity would not pose a problem, but I am curious what the real acceptance criteria should be. Minor diameter as measurable was within spec, but the thread root was kinda jagged, in places that would not contact the mating part. if we reduced the drill size to get the tool to fully form the thread, we got tool breakage.
 
We did some of this on a difficult material,. A-286 for what it's worth. We saw that with the recommended hole size before forming the thread, we got incomplete thread crests. there was like a groove along the crest where the forming tool did not fully deform the material into full and correct thread form. From a functionality and strength standpoint I think that the irregularity would not pose a problem, but I am curious what the real acceptance criteria should be. Minor diameter as measurable was within spec, but the thread root was kinda jagged, in places that would not contact the mating part. if we reduced the drill size to get the tool to fully form the thread, we got tool breakage.

This is how form taps work. They make what is know as a "fish mouth" on the thread crest. There are special full form taps available, but usually it is not an issue.

This is why form taps are not recommended for STI inserts. You can get a false start in the "fish mouth" instead of the actual thread.
 
Thanks. I got 0.287402 or 7.3mm for a drill size with the 5/16-18 roll form tap.

That should work, though the optimal size would be 7.25mm. The closest inch size is either too big or too small. Because the aluminum is so soft and malleable, it should flow well around and not have too much of the form described above. The crest form issue is rarely a problem, other than when it fails to create the correct minor diameter. That issue is most common when you don't use or cannot get the "best size" drill.

Depending upon the application, the failure of the minor diameter to form to within specification standards can often be overlooked in favor of the much stronger threads created by a forming tap. You are essentially forging the shape, and there are plenty of photomicrographs around that show the molecular changes.

Here's a report from the (free) Titex-Prototyp "TEC+CCS" software on how many holes you can expect with a forming tap:

312-18_form_tap_6061.jpg


Expect even more if you use the .002" larger drill.
 
Form taps are nice, but honestly this is 6061. If you can't get 100's of holes out of a cut tap something is very wrong. I have a 5/16-18 spiral bottoming tap TiCN coated that has done 6,000+ holes. Granted that is in 1018 and 12L in a lathe but still. The proper tap (OSG, Greenfield Guhring, Titex, any mid quality tap) in the proper setup, with the proper code should run in 6061 for a damn long time.

If you were doing 100's of holes per part, for weeks, I would pop for EMUGE and they are better, but over kill here. Better off learning on mid grade tooling.

I have seen several drawings specifically forbid form taps due to the funky thread form.
 
I would not use a bottom tap in this situation. They are not meant for initializing threads. Might I suggest the Emuge brand "blue stripe" tap? This is what is called a "modified bottom" tap. It is spiral fluted, achieves full thread at about 2 leads or so, and will eject the shavings from the hole. You can take it right to the bottom of a blind hole if rigid tapping and it is "almost" a bottom tap.
John


Good advice right here. I don't know if the "Blue stripe" is the type for aluminum, but spiral flute, modified bottoming is a great design for blind holes.
 
Roll Form is the way to go whenever possible. I used to run a job with a 6-32 OSG form tap in 1018 that would literally tap 5000 holes before needing replacement.

Also, open up the programming manual for your machine and see what it needs so you can stick the pitch into your code rather than some feedrate that is tied to the RPM. Programming with the pitch lets you change the RPM to optimize easily.
 
The picture you posted appears to be a hand tap. They rarely work under power without breaking (chip build up in flutes). I would suggest a gun tap or roll form tap.
 
Just an update, but I used the rollform tap and it did all 100+ holes perfectly. This is just a fixture plate, so the previous holes were helicoiled and everything works great. Thanks for everyone's help.
 








 
Back
Top