TM-1 rigid tapping -which taps.

[sensph]

Well after a long time saving....and A long time choosing....

I finally bit the bullet and I have bought a brand new TM-1. Should be here in 2-3 weeks. Cant wait.

So I am going through the things I need. Have most things worked out air spindle tooling etc.....

However I have only ever manual tapped threads and I am getting pretty confused about rigid tapping. Not so much the G code ( I have found quite a few examples to have a go at on cnczone and elsewhere).

I am getting confused about which taps to buy? Spiral point , normal ,spiral flute??

I could be asked to perform tapping in most any material but a lot of work in aluminium and 316L stainless.

Can anyone point to some text on which taps to select or give me some pointers.

Many thanks in advance.

Simon

[Geof]

For cutting taps spiral point for through holes and spiral flute for blind holes.

Rigid tapping is simple to do and just needs sequential G84 commands at the different z depths; as far as I know you cannot put a peck command in just a single command.

Make sure both Rigid Tapping and Repeat Rigid Tapping are turned on in the Settings/Parameters (I forget which it is).

[sensph]

Geoff,

Many thanks for the reply.

Aha, I see (re spiral point and spiral flute)

That makes sense.

I couldn't seem to get the picture right in my head.

Simon

[behindpropeller]

Originally Posted by Geof For cutting taps spiral point for through holes and spiral flute for blind holes. Rigid tapping is simple to do and just needs sequential G84 commands at the different z depths; as far as I know you cannot put a peck command in just a single command. Make sure both Rigid Tapping and Repeat Rigid Tapping are turned on in the Settings/Parameters (I forget which it is).

Geof-

Any recommendations on speeds/feeds? I will be running some 6061 parts next week, 1/4-20 and 3/8-16 taps.

Also... I'm pretty sure you said to thread mill anything over 1/2"??

Thanks

Tim

[panaceabea]

I am running a 1/4x28 tap on a part I make quite a bit in 7075 alum and am runnig spindle speed of 600rpm and feed of 21.43 ipm (rpm/tpi) to a depth of .85 blind with no problems.

I just ran a series of 800qty 7/16(aprox) x 16 tapped holes for 3/8x16 helicoils in 1" plate at 1000 rpm 62.5 ipm with no problem . So far 3/4x10 in alum is the largest hole I have done with rigid and it requires a very heavy collet or dedicated tap holder and a shot of oil at each hole instead of coolant, the coolant seems to work fine for me on the smaller holes , but NC taps around 7/16 and up seem much happier with thread cutting oil. I would imagine harder materials would be best with cutting oil regardless of tap size.

Geoff could you give some insight on thread forming taps when working with aluminum? Best to peck ? cutting fluid/lube?

[Geof]

Originally Posted by behindpropeller Geof- Any recommendations on speeds/feeds? I will be running some 6061 parts next week, 1/4-20 and 3/8-16 taps. Also... I'm pretty sure you said to thread mill anything over 1/2"?? Thanks Tim

Be lazy like me; 1000 rpm for everything (up to 1/2"??) because this makes calculating the feed much easier.

On both 1/4"-20 and 3/8"-16 in 6061 I would probably peck something like 0.35" then 0.55, 0.75 to get as deep as I am going.

Did I say thread mill above 1/2"? Could have because the TM is a bit short on power although you can peck one revolution on larger taps and it will work. One thing I do know is that 3/8" NPT brings my Super MiniMill to a full stop.

I cannot comment very much on forming taps because I don't use them; try doing a search because they have been discussed here. One thing I have read is that pecking is pointless on form taps because there is no chip to clear or break and coolant concentration should be increased to 10 or even 15% or something like that .

[Vern Smith]

I use form taps exclusively in aluminum and if you are going deeper than 3 X diameter pecking is a good idea. If you don't the tip of the tap can weld itself to the aluminum with predictable results. 10% coolant is a must for the tap as well as the exposed metal on the machine. I used the manufacturers recommended 5 to 7% at first and put rust spots on one of the vises and busted a couple of taps.

Vern