Internal Thread Tapping Forged Steel (46+ Rockwell Hardness)

Have a look at Gühring it is one of the best tap manufacturers I know. The serial taps are recommended for high strength steels up to 1200 MPa, your hardness corresponds to > 1530 MPa so that only taps with a TiC ot other surface hardness enhancing (plasma) treatment could help. Using the set of 3 taps will any way reduce the load on the cutting edges and allow a higher number of operations but without a surface treatment the wear will be quite rapid.

The Serial tap set is your best option seeing your limitations do not allow for thread cutting with a carbide tool.

If you are using a CNC miller to tap your holes there is a rigid tapping cycle that will feed down 2 or 3 revolutions and then retract to a clearance position to allow for chip removal and also cools the cutting edges of the tap...this is repeated until you reach your desired depth G84. something varies from machine to machine. The same theory behind a peck drilling cycle for deep hole drilling. Remove the chips and cool the cutting tip or edges.

If you do not have rigid tapping you can use a floating tapping head and go in with the #1 tap ( tool # 1) and tap all your holes. Tool # 2 will have the #2 serial tap. Tool #3 will be your finish tap. This process will not crossthread with the floating tapping heads. I use it with 4340 all the time. If you only have 1 tapping head replace the tap at the end of each cycle in the order 1,2,3. just keep track of your sequence.

If you are tapping by hand use # 1 and # 2 and then go in with the finish tap about 3 or 4 threads reverse back out...back in 3 or 4 threads reverse back out and repeat the process. It's a very fine thread be careful...you break one you have to burn it or mill it out with a carbide endmill. Check the finish tap for wear if you hear a sqeaking noise or clicking remove the tap and replace it with a new one...It's about to break.

Lubrication: I use BOELUBE for tapping... blow out each hole after each tapping sequence and fill it with oil. Coolant will work also. Blast it in there.

Good luck!

H1 maybe deemed optimal but an h3 or H5 should be adquate and perform cost effectively.

Oh I agree, the decision to have an H1 Tapped hole is not our work, it is the person supplying the print. I'm not one to go back to those engineers that decided what pitch diameter they wanted this tapped hole to be, and question why they want it. What we can do is ask for more money in order to do it for them since well it will cost more than an H3 etc.

You should also note that bringing up a problem you have, can reveal a flaw they may have made or overlooked. Quite often a question can solve a problem and eliminate mistakes.

I can see that, and i will also add that these parts are for the airplane industry, which obviously has strict specifications, another thing is two separate airplane companies asks for the pitch diameter of this size for the same type of part each needs from us. If two separate, successful, known, airplane manufacturers want the H1 for this hole that's enough for me to just be quiet and do it the best we can.

You may consider starting an H5 then clean up with H1

I recall getting about 8 seconds before dull with carbide .193 drill bits and 12 seconds with HSS using hand drill on Pratt/Whitney casing mods/repairs

I know this is an old thread that I started but just wanted to give some closure.

What we ended up doing that helped is we FINALLY had someone from a tap company that knew what they were talking about. Turns out when there is a callout for an H1 hole it is NOT the same as calling out for an H1 tap!

It's easy to explain on a board but apparently an H3 is technically small enough pitch diameter that it will tap an H1 hole, H2 is a little smaller for better chance and H1 is even better chance of not being oversized.

We started with a custom H1 tap that weren't that great and ended up so that our gages wouldn't even go in so they were tapping undersized, under H1.

Since then we have switched to H2 and we have had no problems since.

Another thing that has helped us get to 40-60 holes per tap is using a machine (cellcon) to drill and tap instead of hand tapping.

Thanks for all the suggestions last year I appreciate it.