tapping deep holes in magnesium/alum

[PaceToolmaker]

Currently I am working on a magnesium prototype which the customer requires 4-40 threads minimum 14 full threads which is equal to 350 deep plus the lead of the tap.My problem is that going beyond -.275 I start breaking taps resulting in scrap parts.I have tried several different styles of taps.Spiral taps seem to work the best but still break beyond -.275.We put in a M0 before the tap to blow chips out of the hole and add oil.Last thing i tried was to tap -.275,do a force tool change,blow out the hole and add more oil and then tap again to the full depth.This method worked pretty good except for that 8 holes out of 64 were bad holes in that a no-go gauge would enter the holes,threads being too big.This was on a Makino S-56.The lead-in of the tap would not always pick up the previous position.The rigid tap must not be accurate enough to tap the same hole twice altho it appears to index every time.Run time on these parts are 4 hours and we have 60 parts to do so i cannot be breaking taps and really do not want to hand tap these parts.

Appreciate any suggestions anybody has with different tap styles/parameters etc...Currently using OSG spiral taps at 250 rpm.We also do a lot of tapping in similar parts with smaller metric taps that we have to do a lot of hand tapping,so really would like to figure something out.Talking with tooling reps has not been much help.

[gcode]

I would try roll form taps if your customer will

allow thier use. If you must use cutting taps

drill or even ream the holes to the high end of the hole tolerance

 

thread tolerance chart

 

according to this chart you can go up to .0939

for a 4-40 2B thread.. if you're going off a drill thread chart you're probably drilling with #43 (.089").

That extra 4 thou can make a differnce.. reaming will also insure you have a straight hole..

Any drill walk at all can be fatal when you're tapping that deep.

 

[ 06-14-2009, 06:11 PM: Message edited by: gcode ]

[PaceToolmaker]

Yes i am drilling with a #43 circuit board drill that drills right on size at .089.I have not tried roll form taps.I think i will try some sample holes drilling at the bigger tolerance that shows on that chart and see how it fits the go-no go.Thanks for the chart link,that will come in handy in the future.

[gcode]

roll tapping is your best bet, but many aerospace

companies will not allow it

[gcode]

Check out this thread.. It starts as a discussion of peck tapping and morphs into thread milling...These guys are thread milling 2-56 holes now

I'm guessing the cycle times aren't real good

but it beats breaking taps in expensive

machined parts made of high dollar materials

 

edit: link corrected

 

[ 06-14-2009, 07:31 PM: Message edited by: gcode ]

[PaceToolmaker]

the above thread link is another link to the thread chart from the previous reply

[PaceToolmaker]

thanks for your help,gives me some options to explore tomorrow...

[heavychevy2155]

Have a look at tapmatic, talk to tech support and see what they recommend. They also have some great info on their web page.

 

www.tapmatic.com

[specv]

"Currently using OSG spiral taps at 250 rpm"

 

This might be your problem, we tap 1500 to 3000 on our makinos. Roll form would probably be best the lead is much shorter also giving you less tap in the hole. I am running a job with M2 form taps and M3 spiral taps right now at the depths that you are.

[88Matt]

quote:

---

roll tapping is your best bet, but many aerospace

companies will not allow it

---

We can't use them at all. roll forming basically leaves 2 burrs on the top of the thread.

[Tim Johnson]

quote:

---

quote:

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

roll tapping is your best bet, but many aerospace

companies will not allow it

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

 

We can't use them at all. roll forming basically leaves 2 burrs on the top of the thread.

---

Chamfer your holes with a center drill. There will still be partial forming at the start of the thread (burr) but it will be below the face surface.

[Bruce Caulley]

Tim, I think he meant on the top of the thread form. Roll forming leaves a douple peak on the minor diameter.

 

Bruce

[88Matt]

Thx Bruce,

 

That is what I meant.

[gms1]

Don't know what kind of control you have on that makino but on our okuma's with osp200 controls we can use E0. in the tap cycle to align the spindle to the same position every time on tapped holes. That way we can retap if necessary.