Is it possible to tap a blinde hole like this?

Higgins909 · Nov 22, 2018

So, the drill is .166 and M5 x .8 if I remember right. The drill corners go to .400" and the tap goes .394" +-.005" Material is a gummy steel. Is this even possible? We then got word that we can drill to .450" max. We usually use a ground screw or plug gauge to measure threads... if that's even the correct way to measure threads. It's in a lathe, there is some kind of tapping head that moves outwards. (I guess so it doesn't break the tap) I found the only Spiral Flute tap in shop, but we usually use a plug or taper tap for most things. They're usually ground down a bit, to more of a bottoming tap. I can't seem to get a clear answer in shop about how to tap a blind hole.

Thanks,
Higgins909

Whysosharp · Nov 22, 2018

Form tap and grind the lead off you can tap to the depth of the diameter. Or get extra particular and drill it then run a .156 EM down to the drill point know you’ve allowed yourself more room for a form tap or potentially a spiral flute tap

Render · Nov 22, 2018

Are you able to Roll (form) tap the thread, we roll all of our M3,M4 and M5 holes, as there is no swarf you can easily tap to the bottom

litlerob1 · Nov 22, 2018

If I understand correctly. You Gage needs to measure a depth of .4", with an allowable drill point to .45". If you're using a 135° Drill your diameter is only .42".

If the first lead on your tap cuts a full thread then it is possible. But likely it doesn't. If your second lead cuts a full thread, then Mathematically you are going to get .39" deep.

There are ways/alternatives. Threadmill is an option. Spiral point Tap as deep as you can a hand chase to depth is also viable. But Tapping that in the Machine is unlikely, and I'd be afraid of busted Taps.

R

NAST555 · Nov 23, 2018

How about flat bottom drill to your max depth? That would give you a bit more space and then roll form as others said. I have used these and they kick butt A Brand ADFO - OSG

I am betting that some "engineer" was involved in this design. I have had one tell me that if I drill 5mm deep that I should be able to tap to exactly 5mm deep :angry:

Mechanola · Nov 23, 2018

You can cut tap but will need a spiral flutes tool that pulls the chips out. There are tap cutters for through bores and for blind bores, hand sets and machine singles. Contrary to popular belief you better tap gummy steel slo[FONT=&quot]—wly so that you have short(er) chips. Else, forming is advantageous. Thread milling is also an option, if you can do that with the machine.[/FONT]

DMF_TomB · Nov 23, 2018

Higgins909 said:
So, the drill is .166 and M5 x .8 if I remember right. The drill corners go to .400" and the tap goes .394" +-.005" Material is a gummy steel. Is this even possible? We then got word that we can drill to .450" max. We usually use a ground screw or plug gauge to measure threads... if that's even the correct way to measure threads. It's in a lathe, there is some kind of tapping head that moves outwards. (I guess so it doesn't break the tap) I found the only Spiral Flute tap in shop, but we usually use a plug or taper tap for most things. They're usually ground down a bit, to more of a bottoming tap. I can't seem to get a clear answer in shop about how to tap a blind hole.

Thanks,
Higgins909

use 2 bottom taps tapping by hand to get the bottom 2 threads. 2nd bottom tap grind end so there is no tap taper on tap. tap by hand to get the last 2 threads. sure you dont want to tap deep with a tap like that. you will feel resistance so you can stop when resistance too high.
.
i ever day use taps where the tip was ground back. recommend hand tapping to bottom of hole. i have busted many a tap getting too close to hole bottom. many cnc over travel tapping. spindle dont stop exactly where programmed but goes a little farther. depends on cnc and rpm. obviously. if spindle turns extra it screws into hole more than programmed

Whysosharp · Nov 23, 2018

This is really a simple problem with which fancy tools need not apply just a regular form tap with the lead ground off and a DR and Endmill no fancy flat bottom drills, threadmills or your in a pickle advise. Drill it flat bottom it and tap it to depth. I think the bigger bit of silliness here is the +/- .005 thread depth callout.

gustafson · Nov 23, 2018

Drill to .4 [corner of drill as you say]
end mill interpolate bottom of hole .45

grind the tit off the bottom of a bottoming form tap

its a little tight that way but not out of control.

yes stupid drawing, both tolerance and depth restriction

Gordon B. Clarke · Nov 23, 2018

Whysosharp said:
This is really a simple problem with which fancy tools need not apply just a regular form tap with the lead ground off and a DR and Endmill no fancy flat bottom drills, threadmills or your in a pickle advise. Drill it flat bottom it and tap it to depth. I think the bigger bit of silliness here is the +/- .005 thread depth callout.

I agree.

A mix of metric and inch so I'll go with metric. A M5 standard thread has a pitch of 0.8mm so the drill should be 4.2mm. 0.166" is 4.22mm so OK.

The easy to remember rule of thumb for tolerancing thread length is ± 2 times pitch so the correct thread length tolerance for a M5 thread should be ±1.6mm (±0.063").

Somebody has just put tolerances on the drawing without knowing or thinking about what they were doing. If I did that on a drawing and the person making didn't contact me to tell me I was stupid (OK more politely than that) he wouldn't become a supplier another time. I'd rather a supplier contacted me 3 times to ask rather than make one mistake.

I can't even imagine how that thread depth tolerance could be verified.

Normal length of thread engagement for an internal M5 is 2.5 - 5mm (0.1" - 0.2").

litlerob1 · Nov 23, 2018

I'm not going to quote all of you guys, but Roll Form Taps have a thread chamfer also. Simply grinding the end off doesn't automatically give you a first full Thread. Note the image below.

Vancbiker · Nov 23, 2018

Gordon B. Clarke said:
......If I did that on a drawing and the person quoting didn't contact me to tell me I was stupid

Fixed ^

I'd call the customer before I quoted a part with threads called out like that. I have had customers tell me to quote it as drawn because other potential suppliers had already submitted quotes without question or they tell me that another shop "has been making them that way just fine".

Whysosharp · Nov 23, 2018

Maybe I’m spoiled but the Guhring form taps we have, have about 1 partial thread at the tip so yes grinding off the first thread gives you a full thread. Gordon maybe they could measure this with a specially ground gauge? Highly unlikely though that anyone would spend that kind of money for a thread that isn’t toleranced to specific fit in UNC terms 1B,2B,3B. Well played on the typical specifications on a metric thread Gordon very educational.

Gordon B. Clarke · Nov 23, 2018

Whysosharp said:
Gordon maybe they could measure this with a specially ground gauge?

There is no logical or practical reason for that tolerance.

You know the saying "There's one born every minute"? It's the kind of thing many could "screw up" if they didn't know anything about threads or the type that hang their brain next to their jacket.

Vancbiker sounds like a sensible supplier.

A test to weed out the stupid? Ask for price on one before you order 1,000,000.

litlerob1 · Nov 23, 2018

That's a funny looking Nut Gordon!!!

Trying to Verify a Thread depth to that tolerance is really a whole different topic, that belongs in the Metrology/Inspection sub-forum IMO. BUT for the sake of my own boredom this fine Friday; if you use a cheater bar on a Thread Gauge you can make it physically deeper. We think to ourselves who in the fuck would use a cheater? But it's really just an extreme example, as a person using the gage can tighten as much or as little as they like and change the outcome by ±.005" pretty easily. But hell, maybe that's the information the OP needs to hear, IDK.

R

Gordon B. Clarke · Nov 23, 2018

litlerob1 said:
That's a funny looking Nut Gordon!!!

Trying to Verify a Thread depth to that tolerance is really a whole different topic, that belongs in the Metrology/Inspection sub-forum IMO. BUT for the sake of my own boredom this fine Friday; if you use a cheater bar on a Thread Gauge you can make it physically deeper. We think to ourselves who in the fuck would use a cheater? But it's really just an extreme example, as a person using the gage can tighten as much or as little as they like and change the outcome by ±.005" pretty easily. But hell, maybe that's the information the OP needs to hear, IDK.

R

From the OP. "Material is a gummy steel." Use a gummy gauge and problem solved! Reminds of trying to by a yard of elastic in Scotland. Keeps breaking when they try to measure it.

litlerob1 · Nov 23, 2018

Gordon B. Clarke said:
From the OP. "Material is a gummy steel." Use a gummy gauge and problem solved! Reminds of trying to by a yard of elastic in Scotland. Keeps breaking when they try to measure it.

Gadamned Scots, you can't trust them anyway, perfected the art of speaking in Circles.

R

CarbideBob · Nov 23, 2018

Thread mill is the only real way and still won't work with a drill point but it will mill the bottom open if programed to do such.
Since you can go .450 deep a flat bottom hole gives you enough room to thread mill it without abusing the front end.
You can grind a follow up form or hand tap back to zero but it won't stay that way very long.
All great if you want to use this "custom ended" tap for 1-4 holes and replace it with another new one.

Is there one-two parts to be done or a thousand?
Bob

Whysosharp · Nov 23, 2018

Bob I don’t think the tap would wear that quickly or fail in such short notice it’s not a 2-56 or 4-40 which we tap by the thousands this way. The DR, flat bottom and tap method works well and despite seeming archaic is the way to go for any part like this. Really how much is an M5 Tap and speed wise it’ll beat a threadmill any day. I’d say the most practical method is what I’ve advised not saying any of you are wrong but this is one of those times where simple is the best way to do it at any quantity. If your doing 1 perfect it’s cheap and easy. Doing 100 perfect you can get consistent results. Doing 1,000,000? Perfect tool costs vs time would be out weighed and a 6-7 dollar tap every 200 parts is reasonable depending on what your mysterious “gummy steel” actually is.

litlerob1 · Nov 23, 2018

I want to believe you Whysosharp, but I don't. There is a part or parts that are missing. For one thing, the time it takes. In general we have to assume at least 3 toolchanges and one feed down and Circular Mill a flat bottom.

I looked up Guhring Form Taps and couldn't find any tech info. on the Thread Chamfer, but they do look right, for what you said earlier......it looks to me like about 3/4 of the pitch, before you get to the full Thread.

I think the process requires more than a single contact to fully form the Thread. But I don't have anything to back that up, it just seems that way.

Is it possible to tap a blinde hole like this?

Aluminum

Cast Iron

Aluminum

Diamond

Stainless

Stainless

Diamond

Cast Iron

Diamond

Banned

Diamond

Diamond

Cast Iron

Banned

Diamond

Banned

Diamond

Diamond

Cast Iron

Diamond

Similar threads