Rigid Tapping and Compression Holders

[n_tydingco]

Rigid tapping allows us to use ...well...rigid holders to tap holes, however, I'm still finding some smaller taps (2-56, 4-40) break even in (mic-6) aluminum after less than 100 holes.

 

This blows when I'm running large parts

 

Does anyone still use compression holders with rigid tapping? I can probably experiment to see if it helps, but I'm under the gun to get some plates done and ready for plating. Also, I saw the thread regarding removing broken taps, but being a holiday weekend, I'm almost a$$ out for finding something to remove a small, 2-56 tap.

 

Thanks.

[crazy^millman]

it is best to usea compression with 95% difference in the tapping verses a 100% you want the compression holder to do it job and if you have it 1:1 then when the tap gets to the end of the hole the compression holder is not pulling the tap out like it shoudl and could make the tap dwell on the top of the thread thus damanging the part and then no good. That si the answer to your question.

 

Now here is a question from me. I would check the machine and see what is wrong with it. Either you have a bad encoder, reversing motor, or the Z axis is not doing its job correctly. Now if you are tryign to do this at aynthing say over 2000 rpms I think you are going to find on most machines better ot use a compression holder anyway. They will do it but using the compression cycles if the machien has it is more friendly to the machien if doing alot of holes. The rigid tapping is a sudden stop reverse and back our of the whole where as the compression is a little nicer to the machien not much but take 1000 holes a day and think about the wear and tear on the machine any thing better is an imporvement in my humble opinion. I have tapped 1000's of hold in Aluminum granted not MIC-6 but you should see the same results if you are using the right taps and have the right amount of coolant mixed in for doing tapping. If I am doing alot of tapping and not using a tap fluid to tap then I mix my coolant 2 times as strong to get lubrication the point of cutting.

 

HTH

 

One other thing you might look at form taps verse tapping the taps are stronger and I have had good results in MIC-6 using them I realize it is a cast material but have had good results.

[MetalMarvels]

I also found that I was breaking a lot of the smaller (0-80, 1-72, 2-56) taps until I began the tap cycle about 0.050 to 0.100 above the part surface. Why it works, I don't exactly know. However, it seems to be working. I was getting only about 50-100 holes before breaking a tap, now I have well over 1000 holes before I start to get a measureable thread gage change when tapping T6061. I am using the VegaRoll taps at the moment.

[n_tydingco]

Thanks guys. I'm using a brand new HAAS VF-9 and was using EXO spiral-fluted 2-56 (GH-3) and 4-40 (GH-5) taps in MIC-6. The HAAS has a programmable coolant nozzle that I have aimed right at the taps and the coolant concentration is at about 8-10% (pretty thick IMO).

 

It's been pretty frustating (to say the least) that 2 hrs.+ of work goes down the tubes because of a "simple" operation. "This has never happened to me before...honest"

 

Nevertheless, I'm doing everything else on this job except tapping the holes which I'll have to probably consider rolling if that'll get me the results I need...and quick.

[chris m]

I'd go for the Hy-Pro NRT Tin coated roll tap in this application, I think. You might want to try a dwell in the hole, too, to give the machine a second to think before backing out...

 

Fast-spiral taps suck when they're that small, BTW, in my opinion

 

C

[?Mark]

Why not consider using thread forming taps...

 

 

Mark

[Keith Graydon]

Roll taps in the sizes that you mention and set the R-Plane to a distance higher than you normally would. say +.25 or so. It allows more time to sync-up.

[Tim Johnson]

I rigid tap at 4000 rpm all day with up to 8-32 roll taps.

A spiral flute tap is a LOT less stout than any other kind of tap. Try 500 rpm and if your tapping ok walk it up until your having problems then back it down 10%. If you can't tap at 500 rpm it's more than likely machine issues.

 

I also never start any tapping less than 1/4" from the part to allow time for the spindle to get in sinc with the feed.

[Brendan P]

quote:

---

Roll taps in the sizes that you mention and set the R-Plane to a distance higher than you normally would. say +.25 or so. It allows more time to sync-up.

---

+1 To that

I had problems returning to my usual Z.1

I now return to Z.3 and have had no problems.

[n_tydingco]

All,

 

Thanks for the feedback I did consider roll taps but thought the spiral fluted taps would be fine. I started the cycle at .250 above the part @ 800 RPM's. Years ago I would use an 8-32 sp-flute tap on 416 stainless and the sucker would last the entire run of 200+ parts.

 

Needless to say, I will order roll taps for the next job.

 

 

[ 06-01-2004, 03:54 PM: Message edited by: n_tydingco ]