Thread minor diameter call out question

[stevo1]

I have not been around in some time now. I hope everyone is doing well.

I have a controversial question for all regarding minor diameter on a thread call out. Let’s use a .625-18 UNF call out on the print. Our customer prints call out the drill size to use for the hole. So the call out looks like so on the print.

.5781 +.015/-.005 DRILL THRU
.625-18 UNF TAP THRU

Question I have gone a few rounds with some colleges on is that the minor diameter of the thread has to be within the .5781 +.015/-.005 call out once the hole has been tapped. The hole tightens up once the tap runs thru and sometimes the .5781 hole is undersized by a few thousands. I always check the hole size before I tap to make sure I am in spec. Once tapped I no longer check it as I would think that the minor should be developed if need be by the tap. Also the fact they call the drill size and do not say that the .5781 is the minor diameter.

The argument with others is they state that because it is called out on the print that you have to maintain the hole size even after it is tapped and the customer should be able to put a pin gage thru and still be in spec.

Anyone know some kind of official standard on this so I can close this discussion? I breezed thru the machinist book and didn’t find anything.

Thoughts??

Thanks,
Stevo

[cybergomer]

I've got a similar situation, the drilled hole before tapping is clearance for a bolt to go thru. The thread itself is just to act as a retainer.

If your concerned about the hole being undersize after tapping, use a bigger drill.

[athack]

Drill hole, tap, run drill through again or ream.


Athack

[ewlsey]

They should be giving a thread class, such as 2B. The 2B controls the pitch diameter.

The .5781 is controlling the thread percentage, which would be around 60%. What would they do if you wanted to use a roll form tap?

I've never seen a thread get rejected if the pitch diameter was good and the thread was within 60-75% engagement. In theory, your minor diameter can never be too small when using a tap, because the minor diameter would be cut be the root of the thread form on the tap. I imagine you would have a lot of problems tapping at 100% engagement

Now you can get in trouble if the minor diameter is too big. That would lead to less than 60% thread engagement. As the thread percentage decreases, so does the strength.

[stevo1]

I've got a similar situation, the drilled hole before tapping is clearance for a bolt to go thru. The thread itself is just to act as a retainer.

If your concerned about the hole being undersize after tapping, use a bigger drill.

I am less concerned of the hole being undersized then I am of the clarification of what the minor diameter should actually be. It also is not always the same. Some holes shrink up and others do not. To unpredictable to just pick a larger drill. I want to be shooting for mean diameter.

Another thing is the customer that I deal with is 100% print 100% of the time. On a $60 part I can live with that but the majority of my parts are $60k per forging.

Drill hole, tap, run drill through again or ream.

Not cost effective.

They should be giving a thread class, such as 2B. The 2B controls the pitch diameter.

The .5781 is controlling the thread percentage, which would be around 60%. What would they do if you wanted to use a roll form tap?

I've never seen a thread get rejected if the pitch diameter was good and the thread was within 60-75% engagement. In theory, your minor diameter can never be too small when using a tap, because the minor diameter would be cut be the root of the thread form on the tap. I imagine you would have a lot of problems tapping at 100% engagement

Now you can get in trouble if the minor diameter is too big. That would lead to less than 60% thread engagement. As the thread percentage decreases, so does the strength.

These are all 3B threads. What you stated as the drill size being the definition of the thread engagement is exactly what I was trying to explain to most. So then my question would be what is the definition of the minor diameter? What dictates it? It is less the fact it can be rejected because of the engagement it is more the question of rejection if a guy tries to put a gage pin thru the hole and it’s less the .5781 tolerance. That is what I am trying to argue at this point.

Thanks for all the input thus far guys.
Stevo

[stevo1]

Bump….
I am still arguing this with others. I will give you a live example that is happening now.

I have a part that calls a hole like so:
.4531 +.01/-.005 DRILL THRU
1/2-20 UNF 3B TAP THRU

We drilled the part and checked the hole size before tapping with a pin and it was at .452 and then proceeded to tap the hole and send the part to inspection. Inspection puts a pin thru the threaded hole to check the .4531 hole size and they can only get a .443 pin thru the thread and proceed to reject the part.

Is if feasible to think that a hole size callout before tapping should be held to size even after tapping????? Is there any kind of standard dimension/machinist book callout/specification/% engagement/ANYTHING that specifies what the practice should be to this callout????

Or am I completely wrong and the above callout means that .4531 +.01/-.005 is suppose to be the minor diameter of the thread when finished tapping?????

Thanks,
Steve

[Chobyn]

Another thing is the customer that I deal with is 100% print 100% of the time. On a $60 part I can live with that but the majority of my parts are $60k per forging.

Not cost effective.

Stevo

Uhm....Does it cost you $60k to run a reamer through the hole after the tap? I am not seeing how it is not cost effective to be sure minor meets their spec.

If they are speccing a through hole as well as a thread, they are expecting a threaded hole that meets that thread callout, as well as a through hole that meets the through hole callout. I doubt the customer cares what size the hole was before you tapped it, he didnt ask you, nor spec it as "prior to tapping". He called out .4531 +.01/-.005 DRILL THRU and 1/2-20 UNF 3B TAP THRU, so that is what he wants on his final part. If there is some conflict between the through hole callout and the minor (which there is here, Machinery's Handbook 24th edition specs a 1/2-203B minor diam to .45370-.4460) then you need to get a clarification as to which he wants held, the 3b spec, or the oversize minor spec, as you cannot exceed the .4537 on minor diam and meet the 3b.

Short version is ream the hole to .450 after tapping and meet both specs, IMO.

[ewlsey]

He called out .4531 +.01/-.005 DRILL THRU and 1/2-20 UNF 3B TAP THRU, so that is what he wants on his final part. If there is some conflict between the through hole callout and the minor (which there is here, Machinery's Handbook 24th edition specs a 1/2-203B minor diam to .45370-.4460) then you need to get a clarification as to which he wants held, the 3b spec, or the oversize minor spec, as you cannot exceed the .4537 on minor diam and meet the 3b.

You are confusing thread class with thread engagement once again. The 3B spec only controls the pitch diameter.

IMHO, if the hole size is good before tapping, and the 3B thread gauge goes after tapping, you are good to go.

[Chobyn]

You may be correct, but I always understood that the class (2b,3b, etc) spec controlled Pitch Diameter, and Minor/Major Diameters. I do know that on the reference materials I have the Minor for a 1/2-20 2b is spec'd to .457-.446, and a 3b is spec'd to .4537-.446 (you lose about .0033 on allowable diameter). If you can back up your assertion with a reference I would appreciate it. Like I said, my understanding could be in error.

[cybergomer]

You are confusing thread class with thread engagement once again. The 3B spec only controls the pitch diameter.

IMHO, if the hole size is good before tapping, and the 3B thread gauge goes after tapping, you are good to go.

So your saying when the customer's QC guy inspects your part and rejects it because the hole doesn't fit the gauge, he's wrong. It doesn't matter how you machine it and at what point you measure the feature, when that part is in your cutomer's hands, that part must meet the drawing spec.

We're also talking about a .015 tolerance here, there should be no reason that size cannot be held. If you can't produce consistent results, check the tools your using, check speeds and feeds, there is no reason why any machine shouldn't be able to hold that size all day long.

[stevo1]

I can’t believe that I missed that spec in the machinist book on the minor size. So yes the print and the spec are conflicting. I will not get clarification on what the customer wants. Even if I was able to they are not going to change the print and the print is what I am held to. The actual hole size tolerance is a default spec that they created to cover anything not tolerance on their prints.

I know they probably don’t care what the hole callout was before tapping it but most of the time when a callout for drill is on the print it is to specify the thread engagement that is desired and that the minor falls where it falls once tapped. I was more or less looking for something that specified if you use this drill size and this 3B go/nogo gage that your thread engagement is met and the hole size specified does not need to be checked. (I was looking to find something that fit my thought process)

Uhm....Does it cost you $60k to run a reamer through the hole after the tap? I am not seeing how it is not cost effective to be sure minor meets their spec.

No it does not. My 60k comment was towards using a larger drill size and that it is not worth trying to predict a larger drill size and have a chance of making an unrepairable feature. At least at this moment I can open them up if they fall small on size in order to meet print. If they are oversized the part is scrap.

Also 60k is the forging not the margin. Some of these parts have 200-300 holes in them. That is a lot of time reaming and eating away at margins so I was hoping to loop thru on a technicality. I have also reamed some holes in the past and endup having to retap some of these holes.

I appreciate the info. That is what I was looking for. Not sure how to approach it yet.

Steve

[ewlsey]

So your saying when the customer's QC guy inspects your part and rejects it because the hole doesn't fit the gauge, he's wrong. It doesn't matter how you machine it and at what point you measure the feature, when that part is in your cutomer's hands, that part must meet the drawing spec.

We're also talking about a .015 tolerance here, there should be no reason that size cannot be held. If you can't produce consistent results, check the tools your using, check speeds and feeds, there is no reason why any machine shouldn't be able to hold that size all day long.

Maybe the OP has some kind of burr on his threads or something, but in my opinion, if the 3B thread gauge goes in, that is a good thread.

What if you were form tapping a blind hole. The drill size would be .4724. You could not get a pin in behind the part to check the hole diameter. Would you break out a machinery handbook and look up the minor diameter and check it with a pin?

[cybergomer]

Maybe the OP has some kind of burr on his threads or something, but in my opinion, if the 3B thread gauge goes in, that is a good thread.

What if you were form tapping a blind hole. The drill size would be .4724. You could not get a pin in behind the part to check the hole diameter. Would you break out a machinery handbook and look up the minor diameter and check it with a pin?

The issue isn't the thread. If the drawing callout was only a 1/2-20 UNF 3B thread, then yes, the information from the Machinery Handbook would apply. But there is a callout for the drilled hole and that callout has to be met.

[Curt B]

Bump….
I am still arguing this with others. I will give you a live example that is happening now.

I have a part that calls a hole like so:
.4531 +.01/-.005 DRILL THRU
1/2-20 UNF 3B TAP THRU

We drilled the part and checked the hole size before tapping with a pin and it was at .452 and then proceeded to tap the hole and send the part to inspection. Inspection puts a pin thru the threaded hole to check the .4531 hole size and they can only get a .443 pin thru the thread and proceed to reject the part.

Is if feasible to think that a hole size callout before tapping should be held to size even after tapping????? Is there any kind of standard dimension/machinist book callout/specification/% engagement/ANYTHING that specifies what the practice should be to this callout????

Or am I completely wrong and the above callout means that .4531 +.01/-.005 is suppose to be the minor diameter of the thread when finished tapping?????

Thanks,
Steve

IMO both whoever made the print and your inspector need to be slapped.


The machinery's handbook gives the following minor diameter tolerance for a 1/2"-20 UNF 3B fit internal thread:

.4460" minimum, .4537" MAXIMUM


If the minor diameter exceeds .4537" the result is absolutely NOT a 1/2"-20 UNF 3B thread.

[SIM]

I get several jobs like this...seems somewhere along the way the guy making the drawings thought he was doing a favor by telling the machinist how to do their job by giving drill call outs. At the time nobody cared about the call out dimension. Then time goes on new inspector, new guy making drawings and that call out becomes law.

One company tells me to just gage the thread to whatever class is called out.
Another company will reject if not 100% to print.

Kind of boils down to what the customer expects.

The again some jobs have required a dowel like pin to fit within and that diameter was pretty important.

[dieselpilot]

You should consult ASME Y14.5M for the drawing interpretation. If they do not follow any drawing standard you're at their mercy. If they do follow a standard, it should be on the print.

Drill and Tap; and calloutformat.txt (Part 1)

This says that the drill note is a procedure. Being that they give size limits however, I think it's binding.

15 years ago as a drafter at an aerospace firm I seem to remember calling out "MOD" and then the minor diameter limits beneath the thread call out. We followed the ASME drawing standard as we had a lot of military work.

Greg

[Gordon B. Clarke]

I'm going to disagree with at least a couple of posts so I'll keep my reply "solo".

When a tolerance class is 1A, 2A or 3A then the major and pitch diameters are specified for an external thread.

When a tolerance class is 1B, 2B or 3B then the minor and pitch diameters are specified for an internal thread.

When no class is specified then 2A and 2B respectively are a given.

Tolerance class 3A has no allowance from nominal pitch diameter. 1A and 2A do. Min. pitch diameter for 1B, 2B and 3B are always nominal pitch diameter.

If a tolerance other than specified within the standard is given by the customer (the standard by the way is ASME B1.1) then that is a special requirement by the customer.

Machinist handbooks are useful but they are not recognized standards. Especially when using older machinist handbooks it should be remembered that standards are revised and updated from time to tme.

Gordon

[barbter]

I'm with Gordon.
Also, the cad man wouldn't have a clue (I expect) that the hole may 'shrink' when tapping, so will expect the core to be to those sizes after tapping.
In other words, make to the print (always safest option).
I would be careful trying a larger drill 1st until you have established the reduction in diameter is not burrs.

[Chobyn]

When a tolerance class is 1B, 2B or 3B then the minor and pitch diameters are specified for an internal thread.


Machinist handbooks are useful but they are not recognized standards. Especially when using older machinist handbooks it should be remembered that standards are revised and updated from time to tme.

Gordon

It was the reference I had on hand at the moment which is why I cited it as my reference in case there was some confusion on the actual 'true' standard numbers. I understand that standards are revised periodically. I was only trying to illustrate that there was a conflict in the stated print dimensions, not give him a standard, per se.