Form tapping 4340 38-41Rc

[jeff]

I have a repeat job of M8 x 1.25 blind holes in 4340 38-41Rc.

Should I just stick with a spiral flute tap or would a form tap be better? I've never form tapped steel, just aluminum.

[Guest]

I have always found harder materials roll form better.....just push your drill to the upper size of the minor dia

 

Course I would threadmill instead if that were an option

[jeff]

I have always found harder materials roll form better.....just push your drill to the upper size of the minor dia

 

Course I would threadmill instead if that were an option

Thanks, threadmilling isn't an option on these parts.

[chris m]

IMO, you are right on the borderline of un-doable with that hardness. We form tap steel and stainless all of the time, and I would suggest the OSG ExoTAP-NRT (NOT the Hy-Pro) for that application. In my experience, if those taps don't come out of the hole, no tap will.

 

Watch the minor dia, the harder material likely won't flow down to the same size as softer material.

 

C

[djstedman]

If you have not already done so, you should probably double check with your customer and any specs on the print, some customers / specs don't allow formed threads since it work hardens the material during forming.

[chris m]

Excellent point!

 

C

[jeff]

If you have not already done so, you should probably double check with your customer and any specs on the print, some customers / specs don't allow formed threads since it work hardens the material during forming.

Good point. 

We decided to go with a cut tap instead of a form tap. 

I contacted Guhring for a recommendation and they also said that Rc is about the limit or may be too much.

Thanks all for the replies.

[crazy^millman]

Good point. 

We decided to go with a cut tap instead of a form tap. 

I contacted Guhring for a recommendation and they also said that Rc is about the limit or may be too much.

Thanks all for the replies.

 

Why don't you threadmill it?

[Sticky]

We form tap 5/8NC in 4340HT, 65% thread. The material is usually around 36-38rc. We are using the OSG XPF coolant through taps. We just use the coolant in the machine, and do not add tapping oil. Works great. They are expensive taps, but they work far better then anything else I have tried in 4340 above 35rc.

 

If going above 40rc, or if you need more then 65% thread I would cut tap or threadmill.

[jeff]

Why don't you threadmill it?

They are long shafts, and we are hanging them over the edge of a Bridgeport using a tapping arm to tap the end of the shaft.

[crazy^millman]

They are long shafts, and we are hanging them over the edge of a Bridgeport using a tapping arm to tap the end of the shaft.

 

Oh. Never mind.

[Mr. M]

If you cannot thread mill on a manual mill, you are not a real machinist. : ]

[chris m]

Yikes; I would be surprised if a Bridgeport had the sack to form tap an M8 in 40Rc material

[jeff]

Yikes; I would be surprised if a Bridgeport had the sack to form tap an M8 in 40Rc material

No, this Bridgeport is just an anchor... .we utilize the table space with a tapping arm bolted down to the table.

http://www.flexarminc.com/index.html

[Sticky]

Yikes; I would be surprised if a Bridgeport had the sack to form tap an M8 in 40Rc material

 

Are you joking? A 24v drill could do that...

 

We have this 304 stainless weldment we do sometimes, we tap and drill a bunch of M6-M8 holes after welding, we use form taps in the 24v drills, works fine.

[chris m]

304 is dogsh!t soft; not sure I see the connection

 

That being said, I am also surprised that the tapping arm will do it; an M8 will pull a pretty good spindle load on a 10HP CNC spindle in material that hard

 

C

[Sticky]

304 is dogsh!t soft; not sure I see the connection

 

That being said, I am also surprised that the tapping arm will do it; an M8 will pull a pretty good spindle load on a 10HP CNC spindle in material that hard

 

C

 

If it does,  it's because the spindle has no torque at the range you are tapping in. M8 form tap in 4340HT is going to be about 30 ft/lbs of torque. HP doesn't mean sh*t for tapping, you need torque. My 5/8 NC forming I do is only using 60-65 ft/lbs of torque.

[ManWithNoName]

Lol, bid the job to a sub-contractor and soak up the xx% while you work on a job that makes money with less hassle =D Hahaha