Advice on Tapping 3/8-24 hole in 316

[r2784c]

I need to duplicate this piece and am not sure best way to tap the 3/8-24 threads in 316 stainless. Pics attached of what I am trying to make (pic 1835 and 1836). Here are the particulars of what I tried so far. End result was tap broke when program reversed spindle to retract tap.

• Material: 316 Stainless
• Drill Size: 0.3543" from Guhring. Hole drilled 1.3" deep from face.
• Tap: 3/8-24 OSG form tap. Model #1400138306
• Desired depth of threads is 1.15". Note this is deeper than the 0.752" of thread length on the form tap
• Haas TL-1 with tension/compression holder (no rigid tapping option)
• RPM = 200
• Manually applied cutting oil to tap before starting cycle
• Feeding and Retracting with G01 commands.
  • 10% reduced feed rate (0.0375in/rev) going in, full feed rate (0.0416in/rev) on retract
  • Z set to 90% of desired depth = 1.035" (Desired depth of 1.15")

All was going well during the feed. When the program commanded the chuck to stop ahead of reversing, it sounded like the tap was binding in the hole. Upon reverse the tap snapped. I have included two pics of the failed attempt (1839 and 1840). You can see discoloration on the outside of the piece near the bottom of the tap. I admit my programmed z travel was cutting it close to the bottom of the drilled hole.

Now that I laid out what I did, which probably has too many errors to count, can you guys provide advice on how I should have done it to be successful?

Thanks

 

[plastikdreams]

I'm not sure a form tap likes 316...

 

[crossthread82]

You can form tap 316 but you have to use a decent lube I like the tap fluid that Emuge sells. That tap likely galled in the bottom of the hole; pretty obvious by the discoloration...it got HOT and grabbed the tap.

I prefer OSG's xpf line of form taps for doing steel and stainless part no. for the tap you need is 1625038245. They have less heat generation and lower tapping torque.

Also be sure you don't run the tap into the bottom of the hole, likely not since it broke on reverse but still double check.

Also check the pre hole diameter your drill is drilling, 0.3543 is right at the bottom of the allowable holes size for a 3/8-24 form tap. Range is 0.3538-0.3580, for SS I like to stick to the higher end of the range so around 0.357-0.358, a T drill is 0.358 which would be a 60% thread, so I'd use that.

 

[r2784c]

Yeah, definitely sounded like it grabbed at the very end. I don't have to use a form tap. Should I consider moving to a cut tap?

 

[Johnhudson]

Moly-D is a good tapping fluid.

 

[DanASM]

Yeah, definitely sounded like it grabbed at the very end. I don't have to use a form tap. Should I consider moving to a cut tap?

Cut tap should be fine. Theres enough meat on it to hold up. Just make sure the material has no work hardening done on any of the surfaces the tap will touch.

Make sure you do not dwell on any cut with the drill prior. Pecking is ok but do not dwell. Use a premium tap, I like OSG material specific taps. Spiral flute bottomming.

 

[r2784c]

Ok. Thanks guys. I will adjust my method and tap and see how it goes.

One follow up question, given I am using a compression / tension holder, do I have one shot at tapping or is it possible to tap 1/2 depth, retract, clean tap and hole, and then go for a 2nd pass to full depth? I am worried the first few threads will get buggered up if I use this 2 pass method.

 

[DanASM]

I have Brown and Sharpe Screw Machines and use "Compression" style tap holders. They extend out when cutting and then spring back as the spindle reverses. It gives the tap some "float" to compensate for any rigidity issues.

I personall have not re tapped a hole like you asked, but my father has. He said it was very common back in the day to do this as a way to clear chips.

Keep in mind the 316 will work harden. The heat is in the chips, and they dont like to break. Which means the heat does go back into the part and hardens it. When actively cutting, the tool stays ahead of the heat as it takes a cut. As long as you stay in the cut, it should cut fairly easily. Its when you dwell, or stop and let the heat catch up to the cutting edge that will give you problems when the next tool comes in.

If you can tap the hole half way and retract, then look at what is left behind after the tap is out. If the surface looks like Chrome, it will be crystalized and hardened. Behind the hard spot it will be gummy again, this can create a "smearing" effect where the tool pushes the hardened part into the softer material instead of cutting it.

This will make threads look horrible, and is the time to sharpen tooling and or try a different approach. Just remember, heat kills tools. 316 SS doesnt take much heat at all to work harden. I think its around 500 degrees F.

 

[r2784c]

Makes sense. I will stick with 1 pass.

If i had to guess where I went sideways it was that I chose a hole size at the min range for form tap and I was aggressive with how far I fed the tap relative to the hole depth. I will correct both and see if results improve.

 

[mhajicek]

Max pilot diameter, good lube, and slow it down. I've gotten hundreds of holes from a form tap in 316, but it was much smaller, I think a #4.

 

[r2784c]

Do you guys think 200RPM was too fast?

 

[crossthread82]

Do you guys think 200RPM was too fast?

Not really 200rpm is only 20sfm which is about right for a form tap in 316

 

[cyanidekid]

Just remember, heat kills tools. 316 SS doesnt take much heat at all to work harden. I think its around 500 degrees F.

this makes absolutely no sense.

yes, heat kills tools, completely separately yes, heat also causes problems in stainless, but "work harden" happens, by definition.. without heat.

AND....FFS! 3/8 -24 has got to be one of the easiest threads to tap! why in the name of Job are you trying to form tap this? fatigue resistance can't be much if a factor in 316, chip evac isn't much of an issue...

P.S., consistent and reliable composition and temper is critical with stainless, use a quality producer with a good track record. use a spiral FLUTE tap.

 

[mmurray70]

Are you sure it burned up from tap? Seems odd for a tap to do that. Im thinking might have been drill overheated in bottom of hole from lack of coolant. That part of hole got hard and then busted tap.

 

[r2784c]

Definitely over heated when tapping. No issues drilling hole.

 

[newtonsapple]

Form tapping is done all the time in 316 for tiny threads in the medical device world.

You are way too tight on the drill at potentially more than 75% thread. Check the OD of the part, you may actually be bulging it out.

For most applications, with a thread that deep, you are going to be fine at 55% thread. The tapping torque should be significantly reduced.

 

[mmurray70]

you look at the part closely in between? Im sure it completed the drilling just fine. Just saying it might have gotten little hot at end of drilling. Problem doesnt show up until you try and tap.

I just cant see how a tap can overheat a part like that. They turn way too slow. Usually if something goes wrong it just snaps or crumbles and thats it, no discolored hot parts.

 

[r2784c]

The part was barely warm to touch after drilling. I didn't notice any discoloration until after tapping, at which point it was too hot to touch.

newtonsapple, the part appears to be bulging now (after tapping and breaking).

 

[crossthread82]

you look at the part closely in between? Im sure it completed the drilling just fine. Just saying it might have gotten little hot at end of drilling. Problem doesnt show up until you try and tap.

I just cant see how a tap can overheat a part like that. They turn way too slow. Usually if something goes wrong it just snaps or crumbles and thats it, no discolored hot parts.

Form taps generate tons of heat b/c they're essentially sliding against the material, especially when the sizes start to get larger i.e. >.25"

 

[crossthread82]

The part was barely warm to touch after drilling. I didn't notice any discoloration until after tapping, at which point it was too hot to touch.

newtonsapple, the part appears to be bulging now (after tapping and breaking).

Yeah, hole was to small and it over-engaged the tap creating a ton of friction, all that heat galled the tap. 55-60% thread is plenty fine in steel/stainless. Save 75% for aluminum.