Problem- Suggestions for Tapping in 303 Stainless

[neilw20]

Originally Posted by extanker59 One thing I've learned about small taps: if you feel it break or hear a chirp like it broke, and when you remove the tap it appears unbroken. Don't believe it! Throw it out and get a new tap.

If it clicks or squeaks you might need a microscope to see the damage, but it will be there !

With the correct tap, it becomes a non-event. Using a jig to ensure the tap is directly over the hole important, and helps to prevent chipping the tap.

Make sure your tap wrench is in good condition so you do not cause any misalignment on starting, and you can 'feel' what you are doing.

I made an arbor that I put in the machine chuck, such that the end of the T wrench hole fits nicely. Without that, the tap won't last any time before you chip it.

[John Welden]

Like Neil just said, make sure you're right over the whole with the tap.

Centerdrill/spot
drill
tap

than move to the next hole. When everything is lined up perfectly it should go just fine. Get one of those spring loaded tap center things to prevent you from snapping the tap with side load.

What you're asking to do is really no big deal. Practice in a scrap piece so you can get the feel for it and find out if you're doing something wrong. With proper technique there is nothing to worry about.

I'd say the biggest mistakes are not being over center, bottoming the tap out, using a junk tap, and simply snapping the tap off because you put side load on it.

[neilw20]

This is just my opinion. I might be way off track, but it works for me.

Stainless steel is funny stuff and easy to work with once you understand a few rules.

It is actually quite ductile, and this causes problems if the tool or cutter is not extremely sharp. When you attempt to cut the material pushes out of the way if the cutter is not dead sharp. Once the cutting edge has the slightest shiny rub mark (and you need a magnifying glass the damage is so tiny) then the cutter/tap will push the material away, start to work harden and damage the cutter further.

Stainless steel is a poor conductor of heat, so it takes very little extra friction to damage the cutter. I think that's why high speed steel does not work well. Lots of coolant can help.

High speed steel and Tin coated cutters don't seem to survive well. It would appear that it only takes a small amount of the base material to embed in the cutting surface, then you don't have the hard edge any more and then the friction and rubbing kill it. All in the blink of an eye usually.

I have found 8 degrees is just enough clearance on the cutting face, and 9 degrees perfect. 10 degrees is too much.
Because the clearance angle is high, the cutting material needs to be quite strong to resist the forces on very sharp edge.

I run carbide cutters for 4 hours, then they need to be resharpened until all the shiny damage is gone.
Once a cutter or tap starts making any noise or you get chatter (that's noise) then the rot has set in.

I have tapped over 100 M4 holes with an intermediate tap and it still works OK. Very important to use good quality thread cutting lubricant.
I hate tapping M3 holes and smaller.

Similar rules apply to titanium which is almost identical in thermal conductivity.

[All4fun]

Hi all,

I want to thank you fine gentlemen for the ideas, insight and experience. I have modified my game plan with the input I have gotten. Here's the new (hopefully improved) plan:

I modified the design so all the holes will be thru holes and tapped thru all the way (no blind holes to tap). Still tapping 4 holes in M4 and 5 holes in M6. I will use Moly-Dee as the cutting fluid which a friend has kindly loaned me. I have obtained new OSG taps. And last but not least I have a way to make sure the tap is started right on center on the hole. I'll be doing the drilling and tapping on a Bridgeport.

The part I don't have worked out yet is if I want to drill the holes a bit oversize? Hmmm.... suggestions are welcome gentlemen.
...

[djr76]

Originally Posted by All4fun Hi all, I want to thank you fine gentlemen for the ideas, insight and experience. I have modified my game plan with the input I have gotten. Here's the new (hopefully improved) plan: I modified the design so all the holes will be thru holes and tapped thru all the way (no blind holes to tap). Still tapping 4 holes in M4 and 5 holes in M6. I will use Moly-Dee as the cutting fluid which a friend has kindly loaned me. I have obtained new OSG taps. And last but not least I have a way to make sure the tap is started right on center on the hole. I'll be doing the drilling and tapping on a Bridgeport. The part I don't have worked out yet is if I want to drill the holes a bit oversize? Hmmm.... suggestions are welcome gentlemen. ...

No, stick with the 60% + range, OSG VA3 spiral point plug taps?, you should not have a problem with the through holes, Ill tap holes all day long with those taps without a tool change out. Dont be scared of 303 stainless, its a pretty tame material and will tap like its going through butter.

[John Welden]

Originally Posted by All4fun Hi all, I want to thank you fine gentlemen for the ideas, insight and experience. I have modified my game plan with the input I have gotten. Here's the new (hopefully improved) plan: I modified the design so all the holes will be thru holes and tapped thru all the way (no blind holes to tap). Still tapping 4 holes in M4 and 5 holes in M6. I will use Moly-Dee as the cutting fluid which a friend has kindly loaned me. I have obtained new OSG taps. And last but not least I have a way to make sure the tap is started right on center on the hole. I'll be doing the drilling and tapping on a Bridgeport. The part I don't have worked out yet is if I want to drill the holes a bit oversize? Hmmm.... suggestions are welcome gentlemen. ...

No need to go oversize. You're going to be amazed at how easy this is going to be. You've got a good machine, good fluid and good tap. The rest is just drilling a straight hole without turning the part blue.

I'd even power tap those suckers if I had a lot to do. By hand is too much work, takes too much time.

like I was saying before, do a few practice holes and make sure your setup is good. When I was an apprentice I had to drill and tap 100 #4-40 holes in a block. Threads had to be nearly as deep as the tap would go. If I broke one I had to start over. This was in 7075 aluminum, power taping in a bridgeport. I think I started over a couple of times. The hard part was doing it with a couple of mean old mold makers watching over your shoulder and asking what's taking so long.

[mc-motorsports]

Spot drill your holes to make sure the drill centers nice, definately don't go under-size. Thru holes, OSG taps, threading oil, proper fixturing, no problems.

Don't be afraid to power tap, but use a collet or precision collet holder like a ER-16, drill chucks usually have too much run-out. I wouldn't chance it.

MC

[All4fun]

Originally Posted by djr76 No, stick with the 60% + range, OSG VA3 spiral point plug taps?, you should not have a problem with the through holes, Ill tap holes all day long with those taps without a tool change out. Dont be scared of 303 stainless, its a pretty tame material and will tap like its going through butter.

The OSG taps I got are HSS, not the VA3. I may have got the wrong ones for the job. Hopefully I am not headed for a problem?

Originally Posted by John Welden No need to go oversize. You're going to be amazed at how easy this is going to be. You've got a good machine, good fluid and good tap. The rest is just drilling a straight hole without turning the part blue. I'd even power tap those suckers if I had a lot to do. By hand is too much work, takes too much time. like I was saying before, do a few practice holes and make sure your setup is good. When I was an apprentice I had to drill and tap 100 #4-40 holes in a block. Threads had to be nearly as deep as the tap would go. If I broke one I had to start over. This was in 7075 aluminum, power taping in a bridgeport. I think I started over a couple of times. The hard part was doing it with a couple of mean old mold makers watching over your shoulder and asking what's taking so long.

Thanks. I do have a practice piece to make sure I have the setup right before I work on the final workpiece.

Originally Posted by mc-motorsports Spot drill your holes to make sure the drill centers nice, definately don't go under-size. Thru holes, OSG taps, threading oil, proper fixturing, no problems. Don't be afraid to power tap, but use a collet or precision collet holder like a ER-16, drill chucks usually have too much run-out. I wouldn't chance it. MC

Sounds like strong concensus not to go oversize on the holes.

I appreciate all the responses gents. It has been very helpful. This is a great forum. Cheers.

[mc-motorsports]

Originally Posted by All4fun The OSG taps I got are HSS, not the VA3. I may have got the wrong ones for the job. Hopefully I am not headed for a problem? Thanks. I do have a practice piece to make sure I have the setup right before I work on the final workpiece. Sounds like strong concensus not to go oversize on the holes. I appreciate all the responses gents. It has been very helpful. This is a great forum. Cheers.

I didn't vote to not go over, I voted to make sure you don't go under! A couple of thou will make a difference... Your call.

And take those taps back for sure if they are just HSS. Atleast make sure, the taps you want should have vanadium in the chemistry. Night and day difference.

MC

[djr76]

Originally Posted by All4fun The OSG taps I got are HSS, not the VA3. I may have got the wrong ones for the job. Hopefully I am not headed for a problem?

If they are designed for stainless, be not afraid. 303 is relatively soft material, its gummy, not as hard as ppl tend to believe. Now if you were tapping 440C or 304 Plate, then I would be concerned with exact tooling.

[Rich Kay]

My personal experiences with tougher stainless 304's 304L's is that if the thread percentage is not specd' it is simply good insurance (but not necessary) to drill a tad oversize. I drill and tap anywhere from 30 to 100 holes larger dia. (3/4-10 tap and up) in a given day in some really challenging castings such as Titanium, Ferrilium 225, HC250, Nitronic 50 to name a few of my pesky materials. I often have a $60,000 Titanium 36" casing on my machine, and "if" I snap a tap, that's a BIG timely setback to correct! I've recently been graced with operating a brand new Yama-Seiki VMC 1600, and my new favorite tap method is rigid PECK TAPPING !! What a problem solver peck tapping has been for me. I can use inexpensive HSS gun taps with ease... I add in a Q.3 peck value and no more stress on me ! Everyones situations and circumstances are different, I just though I would post up my thoughts. Good luck,
Rich

BTW: Hello everyone, my name is Rich, and I am a tired and weary CNCaholic

[extanker59]

Hi Rich
You have come to the right place.
Chris