[stovepipesteve]

material A36.
machine is a VF3,30 horse, gear driven. 50 taper.
tapping 2'' deep. The tap is 4 fluted.
im thinkn of starting out about 100-125rpm.
ill be holding the tap in a collet so im worried that it will slip in collet running the torque its going to require to tap 2'' deep.
any thoughts would be great.
thanks.

[Donkey Hotey]

Edit: I'm a moron. I read the original post as a 3.0 mm tap, 3" deep, not a 30 mm. Never mind. That's a huge tap. Ram that sucker in there.

[dertsap]

the collet will probably slip pecking or straight tapping
your best bet is to ditch the collet holder and make a sleeve to fit the tap into a sidelock ,other than that i cant see any reason you can't tap 2" deep if its spiral flute , ive done it many times with near the same or larger dia taps to more depth , chances of breaking the tap is slim to non if it is of any quality ,
if your tapping multiple holes then i would suggest monitoring the tap in between holes and watch that your not building a bird nest around the tap because it will do damage

[Jason3]

Greg - you had me worried there I thought I was a bit of a small thinker for a while - wow, I thought. M30 is a small tap. He must do some BIG work!

Jason

[Donkey Hotey]

Yeah, I was looking at some really small taps the other day. I read the post and wondered how sombody would push a 3.0 mm tap through 17D worth of steel. :withstupi

[Excelmachine]

How about thread milling it?

[stovepipesteve]

well i went in for the kill today and ran the big M30x3.5, 4 flute, bottom tap 2 inches deep,3 times.
I used a speed of 120 and a feed of 16.5354. i flooded it with coolant and let her rip, it did awesome. Im holding it in a large collet so ill keep an eye on the holder cap loosening or slippage.
Thread milling was not an option due to cost and hard to find mill body to insert type and ive never thread mill before, i would love to master it though.

[ttieuli]

You can try Vardex thread mills. I've thread milled some pretty big threads with them. Vardex has software that will write code you can cut and paste.
It's really very easy!:cheers:

[PBMW]

You could have bought two thread mills for the price of that tap....
And it would do the job nicer and faster. Not to mention lasting longer....

[dertsap]

And it would do the job nicer and faster. Not to mention lasting longer....

nicer ?
threadmilling will take a lot longer amount of time if there are multiple holes

[Ronniewhite70]

I know this is an old thread but I'm tapping some M30 Holes 2" deep with an OSG spiral flute. Had a lot of trouble with the threads gaulding. Opened the minor dia up a little and that helped, but occasionally the tap will really trash up a few threads? Generally at the bottom of hole. Using a floating head. Could a rigid tap cycle help with this? Thanks

[Machineit]

I know this is an old thread but I'm tapping some M30 Holes 2" deep with an OSG spiral flute. Had a lot of trouble with the threads gaulding. Opened the minor dia up a little and that helped, but occasionally the tap will really trash up a few threads? Generally at the bottom of hole. Using a floating head. Could a rigid tap cycle help with this? Thanks

What size hole are you using? What as lubricant?

[Ronniewhite70]

I've got the hole at top of tolerance 26.768(1.052). Using a semi synthetic mixed at 5%...rpm of 110

[angelw]

I know this is an old thread but I'm tapping some M30 Holes 2" deep with an OSG spiral flute. Had a lot of trouble with the threads gaulding. Opened the minor dia up a little and that helped, but occasionally the tap will really trash up a few threads? Generally at the bottom of hole. Using a floating head. Could a rigid tap cycle help with this? Thanks

Hi Ronnie,
When tapping to the bottom of a blind hole, rigid tapping is preferable if the only floating holder is of a standard type without any length positioning capabilities. Tapping to the bottom of a blind hole with a Floating Holder is reliable by using the type of holder that will allow the tap to stop rotating whilst the holder freewheel with the spindle around the stationary tap. In use, the Tapping Cycle has a Dwell specified when the Z axis reaches the Z coordinate of the cycle. Because the Z axis is stopped but the spindle is still revolving, the tap continues to feed, thus extending the floating holder until the internal drive finds the freewheel zone (usually an annular groove in which a drive dog is able to freewheel). After the Dwell period, the spindle will reverse but the tap remains stationary until the drive engages again as the Z axis feeds in the reverse direction.

The best method of all, in my opinion, would be to Thread Mill a thread of that size using a multi-tooth Thread Mill. Start at the bottom of the hole Climb Mill to the top leaving the swarf behind,

Regards,

Bill

[Machineit]

I've got the hole at top of tolerance 26.768(1.052). Using a semi synthetic mixed at 5%...rpm of 110

Didn't see the material, but you can open the hole up more. Your hole size if for a 75% thread at no more than one depth of the tap, (about 1.180"). When tapping deeper hole you need to go larger and get into the 55% range or you will have issues.

For example, a 1 3/16" x 12 tap has a minimum hole size of 1.097" for a short hole, but at one and a half to twice the tap width depth, it is a maximum of 1.120." Open up your hole and it will be much better.

In that size it wold be better to thread mill, but that mill would be very expensive.

Mike

[Ronniewhite70]

Thanks everyone. I do a lot of thread milling. But there are 22 holes in each part and 33 parts to run. I have the minor dia opened up to the top of tolerance. May just have to thrd mill and sacrifice a little machine time..

[Ronniewhite70]

Attachment 237398