Thread Forming Question

[Namliek_J@TheeCircle™]

I am using a Guhring 10-32 Thread Forming Tap in Al. 6061. When I found the calculation, I determined that my drill size was a number 16. Is this right? Where can I find a good reference for determing thread forming tap drill sizes?

[Namliek_J@TheeCircle™]

Also, what kinds of feeds and speeds should I be using? I am new to using thread forming taps.

[Don S at Barefoot CNC South]

You want to drill the hole to the thread pitch dia. I always ran at the same speed I would for a cut tap. When form tapping hole size is important.

[John13]

Look here this is where I get my tap drill sizes for form taps(jarflos)

I run same speeds and feeds as cutting taps as well

[Namliek_J@TheeCircle™]

is there a special formula that you use to calculate threading speeds and feeds? what is the basis that you use?

[Namliek_J@TheeCircle™]

i see that in the link that john sent me there is a speed table, what kind of surface feet should i be running?

[John13]

I let Mastercam calculate my speeds and feeds.

[Namliek_J@TheeCircle™]

mastercam says I should be running like 1400 rpm, but when i go even 1000 it pulls the threads right out of the hole.

[John13]

Mastercam for me says 1407 rpm with a feedrate of 43.980263.

 

 

I have a HAAS conversion formula chart here that gives a formula for mill tapping feedrate..

 

IPM= 1/TPI x RPM

 

IPM= 1/32x 1407= 43.96875

 

 

Also doublecheck and make sure you have TAP G84 selected, I don't know how often I've let it at drill and screwed up holes.

[Kannon]

quote:

---

Also doublecheck and make sure you have TAP G84 selected, I don't know how often I've let it at drill and screwed up holes.

---

yeah, I hear ya on that one... taps dont like the peck cycle either!

[John13]

I'm glad that's not just me that's done that.

[Namliek_J@TheeCircle™]

i keep breaking stupid taps, i think what is happening is that my machine begins to back the tap out before it is actually ready too, and it puts stress on the taps and they break.

[TFesta]

What is the size of your machine/spindle? Does it have rigid tapping? A lot of the older machines can't even come close to the new tapping speeds. The spindle tends to lag behind and are slow in reversing the spindle. On the big machines I use 20sfpm, yeah it's slow but we don't do production so it's just to get the job done. Just keep stepping it up till you find your limit if you want.

[Namliek_J@TheeCircle™]

I am running a HAAS VF-4 that is 12 years old. It has rigid tapping, but like you said i think the spindle is laggin behind.

[Kannon]

just curious..

Do you have a "J" in you tap line command?

with rigid tap it allows you to go out of the hole with the tap quicker then enter. For example a J2 in the command line will go twice as fast out as in, J3 three times as fast, all the way up to J9. I was just thinking if it was in there it might be torqueing the tap on the reverse speed increase if you had it in there.

[Rick Henrickson 65]

For thread forming it is not quite cut and dry on drill sizes depends on H or D number tap and speeds and feeds are important try to keep them at even numbers. Equaly important id coolant and concentration level of the coolant. Last does your machine have rigid tapping and are you using a compression retention type of holder.

P.S. Balax has an online catalog you can print out they have a great tech. section.

[?Mark]

J.Keilman, can you post a code?

It's either wrong code, or your machine can't handle rigid tapping at those speeds.

[Gary]

Mastercam will adjust feeds based on the tap you pick. Just enter a lower rpm and it will update the feed. Just click in different box. I would slow one down see what it does then step up from there.

[Tim Johnson]

I tap a 10-32 at 4000 rpm. (max tapping speed) I figure my alum tapping speeds at 250 sfm. I use a No.16 drill for holes at or deeper than 2x dia and a No.17 for holes less than 2x dia.

[Namliek_J@TheeCircle™]

i dont have a j on my tap line, i am just got done using a DTM tapping head and just did 357 holes in SAE 1141 at 1200 RPM and 60 inches a minute with no broken taps. i had to stop, ran out of holes.

[crazy^millman]

Up my post count freaking double post.

[crazy^millman]

I would look at a Floating holder for the tap that should make up any problem you are seeing in the spindle and will keep you have having to spend big bucks if the machine has a problem and would require fixing it.

 

HTH

[?Mark]

quote:

---

1200 RPM and 60 inches a minute

---

If that's for 10-32 tap, then the numbers don't add up

[crazy^millman]

No Mark I think he was making a referecne to another job is all not being spefic to that tap in question.

[Gary]

I think a haas will only tap up to 100 ipm. Thats what I read anyway.