[Vern Smith]

I use a 36 if it's a through hole but back off to a 35 for blind holes. 90% of what I do are my own projects or products so I'm not constrained by other's specifications. From what I read on this forum, this is a luxury most of you don't enjoy.

I'm using 10 to 12% coolant concentration which I think plays a big role with small taps in Alum. I also spot drill anything under .125.

Before you turn your shop upside down just try the spiral point, I think that will make the difference. Some say the form tap will work without drilling a hole first.

Vern

[Ken_Shea]

Paul,
While I agree with Eurisko with regards to Compression Tap holders, don't be too quick to write them off. I have three different makes here and all three are adjustable for compression movement, mine are set to none. As I recall you can adjust these too tight and then are unable to insert / release the tap holder insert.

My approach, admittedly a bit wimpy, is tapping a slow (200) rpm using tap-Magic and blowing the chips off (if using cut taps with each retract again adding a bit more tap-magic. With the 200 rpm and a plunge clearance .5 or above there is plenty of time for this.
I realize this would not be all that practical for production but my tap breakage is down to almost none.

[LYN BYRD]

USE A FORM TAP. I RUN A JOB 3/4 ALUM, 6-32 HOLES, TAPPED 11/16 DEEP, AND HAD THE TROUBLES THAT YOU HAVE LISTED. I CHANGED TO AN UNCOATED FORM TAP AND HAVEN'T LOOKED BACK.
HOPE THIS HELPS.

[Dr Honda]

I give a vote to forming taps. I ran some parts a few months ago using an 8mm forming tap, and did over 600 holes with it.

But with that said, I just did a fixture with 3mm taped holes using a gun style, spiral point, and didn't have a problem. I use ER collet holders for al my taps. Personally, compression holders allow movement, which can break a small tap. If the machine can do rigid... then it should be RIGID!

And needless to say... a good tap is key. (Greedfild should be good though)

Good luck

[duenow]

Form tap, get RPM up to 1000, spot 90 deg, drill .125. Balax taps. I have tapped 1000 6X32 holes in SS on a lathe (but used oil) with 1 balax tap tin coated, then changed the tap, was a 5000 part run, these were blind as all lathe bar work work is.

[fourperf]

when you form tap on a mill do you still use a rigid taping cycle and treat it the same way or do you do something different

mark

[sundy58]

I broke a couple hundred dollars worth of taps (cutting and form with the correct size drill) working with the Haas customer service engineer. Super helpful and knowledgeable. I use Feature CAM and let it set the feed and speeds.

Once I set the rpm to 100 or below I haven't broken a tap. 2/56 and 4/40 are what I tap most of.

This is not a production shop so I can afford to go slow.

I have a TM-2 and use flood coolant with cutting taps.

[duenow]

when you form tap on a mill do you still use a rigid taping cycle and treat it the same way or do you do something different

mark

Rigid tapping the same as using a cut tap no chips to worry about & you can run faster. Form taps like faster. One thing you should spot 90 deg a little deeper as the form tap will "pooch" up the thd more.

[duenow]

I broke a couple hundred dollars worth of taps (cutting and form with the correct size drill) working with the Haas customer service engineer. Super helpful and knowledgeable. I use Feature CAM and let it set the feed and speeds.

Once I set the rpm to 100 or below I haven't broken a tap. 2/56 and 4/40 are what I tap most of.

This is not a production shop so I can afford to go slow.

I have a TM-2 and use flood coolant with cutting taps.

If you have to run at 100 something is wrong with your machine or your feed.

[Vern Smith]

Remember, form taps take a much larger drill size, 1/8 for 6-32.

Vern

[Dr Honda]

tapmatic's website has a good drill chart for roll (forming) taps.

Here:

Std.

http://www.tapmatic.com/pdfs/01_drillselectionchart.pdf

Metric

http://www.tapmatic.com/pdfs/02_metricrollformchart.pdf

[Ken_Shea]

when you form tap on a mill do you still use a rigid taping cycle and treat it the same way or do you do something different

mark

Mark,
If Rigid tapping is available there is no good reason not to use it, the use of a tapping head is also OK.
Nothing special other that what has been mentioned, drill sizes are different then for cut taps.

Maybe one other little point in using form taps is that you will want to spot drill a little deeper than normal to compensate for the the little mound of metal that will be created at the entrance as the metal is being displaced.

Ken


OOPS.... missed duenow's post, oh well

[fourperf]

thanks Ken. I do rigid tap but will try form taps.

They sound like the way to go.

Thanks all

Mark

[kel1]

You do want to tap smaller holes as fast as possible as you will have less tap breakage using this method as long as you use the proper center or spot drill, drill, then tap. I have been using FORM taps for years now and have had excellent results rigid tapping on many different CNC Mills and Lathes with minimal breakage.
You are tapping a 6-32 thread .2 deep and you have a .6 deep hole and you are breaking taps ?? I can say this about the 6-32 thread, it used to be one of the hardest holes to tap without breakage but things have changed. You are only going .2 deep though and you have lots of clearance underneath so it doesn't make sense for you to be breaking taps.

My 2 cents worth is your hole is out of position to start with if no center or spot drill were used or if the hole was in the right spot was the hole measured for size ? was the hole deep enough ? Blah Blah !

The bottom line is that if the hole was in the right location, it was the correct diameter and the correct depth and you are using coolant you shouldn't be breaking hardly any taps of any size if you use the correct tap and yes I do highly recommend Form taps because they are stronger and you can relieve them a bit to bottom tap with. Even if you use a spiral flute tap or a spiral point tap they shouldn't break in aluminum at that depth.

I would hold a 6-32 tap in a solid holder. I dont recommend using the floaters for much accuracy and you do increase the risk of tap breakage.

The only other thing that came to mind was that maybe the timing of the spindle speed to the Z axis movement is out a bit. Encoder ? Maybe a paramater? Highly unlikely though.

Good Luck !

Kel

[pmurdock]

once again thank you for all the suggestions! very helpful thread! I'm out of town for a few weeks, but will return and will report the results of my tapathon..

cheers,
Paul

[littlerobb]

I know I amthe odd man out here but I am all about spirals. I agree with Kel though it sounds like you have an alignment issue, maybe a dinged collet? Maybe a little dullness on the drill. A couple tenths on that diameter is going to effect you alot