Thread Depth Specifying - Sanity Check Requested 3

[KENAT]

When specifying the depth of threaded holes I got in the habit some time back of usually specifying something like:

“… .25 MIN FULL THREAD”

or

… “.125 MIN FULL THREAD DO NOT BREAK THRU”

Unless function requires a maximum as well as minimum depth.

To my mind this meets the real functional requirement without requiring extra inspection to check the max full thread depth. I find this especially useful as when using automatic call outs our CAD system puts the thread depth to the same no. decimal places as the thread diameter, so if you have a 3 DP hole dia (as is typical) you by default end up with 3 DP depth, which on our tol block is +-.005 so is rarely warranted. To change just the depth to 1 or 2dp you have to make the dimension non associative (or have some other kluge) and even then I’d think it rare that +-.010 or +-.030 is really required.

Also if I have a hole that goes from a face and intersects with another hole (common here as we have quite a few pneumatic manifolds or similar) I’ll say something like:

…THRU TO Ø.201 HOLE

I just had a designer argue both of these with me, his main objection being that these notes take up too much room (this on an E print). When I said about putting max/min increasing inspection he countered that we don’t inspect this stuff anyway. While probably true I find it a poor argument, especially as we are moving to outsourcing to different vendors (as mentioned in previous post) where inspection may become more significant. Obviously on the holes that go thru to another hole, there isn’t usually a hole depth left to measure.

So, any thoughts on if I’m right, he’s right or there’s some better way I’m missing. Please don't get hung up on our ridiculous inspection situation, though of course it is pertinent to a point.


KENAT, probably the least qualified checker you'll ever meet...

 

[btrueblood]

Kenat, I would agree with your order of precedence. Sometimes, those are unattainable "goals", just like sometimes driving a truck over unimproved roads, or worse, is an excersize in survival - just get through another day.

Whitmreegt, Ah - thanks - I was not seeing the alternate possibility of a cross hole smaller in dia. than the thread. But, in that case, a section view would show the bottom of the hole, and could also be drawn to show the bottom of the threads, so that both could be clearly dimensioned.

 

[wallyd999]

Kenat I agree you have he right call outs on the thread depths. I would however call out a depth to a cross hole even it is a reference dimesion.

as for Matt Lorono why are you having the guy on the floor going to look up some other piece of paper, chart or spec to find out what drill size is needed. If he has to look it up then the inspector has to look it up as well.

If you have it readliy available give the people all the information that they need.

 

[ewh]

Calling out the drill size for a tapped hole is redundant. Everything about the thread (except perhaps the depth) is in the thread spec, which the machinist should be familiar with. If you are going to vary from that spec, then you spell it out. A primary rule of good drawing practice is to only define the part, NOT tell the machinist HOW to achieve something (unless it is not covered by a specification and is critical to the function of the part).

Believe it if you need it or leave it if you dare. - [small]Robert Hunter[/small]

 

[KENAT]

Thanks for the re-affirmation on the thread depths wally, and while I still don't completely buy it I will from now on give depths for intersecting holes.

However, I'm affraid I'll have to disagree with you Wally and side with fcsuper & ewh on the tap drill issue.

When working to ASME Y14.5 (and general drawing convention anyway from previous employers) you specify the finished part. As such you specify what the finished thread is. You do not specify what tap drill dia to use. In fact in the ASME series where it talks about how to specify threads on the drawing, no where that I know of does it say to indicate the tap drill. I know a lot of people/places like to do this though.

Now if we extend the tap drill beyond the threaded hole we will normally define that dia but often we deliberately choose a smaller dia than either the tap drill or thread minor dia to avoid confusion (arguably at the expense of an extra machining step).

KENAT, probably the least qualified checker you'll ever meet...

 

[KENAT]

"If he has to look it up then the inspector has to look it up as well. "

Forgot to say (unless you're talking about where the tap drill continues on past the thread for vac holes etc) the hole created by the tap hole is no longer there, it has been threaded, so the inspector can't inspect it anyway. In fact isn't that another reason not to have tap dia on the drawing?

KENAT, probably the least qualified checker you'll ever meet...

 

[wallyd999]

I will give somewhat on this issue. If we are doing tooling then yes all I need do is tell them the thread required (plus in size it heat treat is required) and min thread depth along with the drill depth.

When I'm processing a job I do not want the operator or the inspector or the tool setter to look up the size required or the gage required or any of the above. Some of customers have their own set of specs that alter the standard sizes of most threaded standards (and other features). I as a process eng would insist on this as the machine time that is being wasted would be a good deal. Why have a production guy look up some minor issues when the total lot would be 10-40 pcs, every 2 years. When it can be documented once and frozen.

Once again it is how far do you need to take the processing of the detail in you facility. In our case we deatil everything and if we miss it we do a formal revision change.

 

[ewh]

If the customer alters the thread specs from standard, then by all means note that on the drawing. If not, then only specify the thread desired, not how to achieve it.
If you are concerned about the machinist taking too much extra time looking up standard specs, then include the sizes on the work instructions, not the drawing.

Believe it if you need it or leave it if you dare. - [small]Robert Hunter[/small]

 

[KENAT]

See ASME Y14.5M-1994 1.4(f) to support what ewh put.

It's not that I don't have any sympathy for what you say wally but where do you draw the line? 14.5 draws a line, it's up to individual organizations preparing drawings to decide if they use that line, just don't tell me you're fully 14.5 compliant if you aint;-).

KENAT, probably the least qualified checker you'll ever meet...

 

[KimBellingrath]

If you want to control threads accurately, you don't do it by telling the machinist what drill to use - you insoect with a thread gage. Period. Drawings should not be confused with process sheets. Telling someone which drill to use does not ensure the thread form. Do you want to measure a drill or inspect threads? It's a nicety to help the shop personnel but not part of the function of a drawing which has a sole purpose of defining the final condition of a part. Use a mil spec or such to describe the thread and let the shop personnel provide it.

"If he has to look it up then the inspector has to look it up as well. " Why would the inspector need to know what drill you used?

 

[btrueblood]

Kim, ewh, and KENAT: regarding not specifying tap drill sizes, what do I do if I want to control the depth of the tap drill hole, independent of the thread depth, e.g. to prevent break-thru? Is a callout of the form "DRILL POINT DEPTH XXX MAX" or some such, i.e. not specifying the drill diameter, acceptable? Or is the term "DRILL" not allowed, since it implies a process (drilling) and as such is verboten per the standard which says don't specify how the part is to be made...

 

[KENAT]

This is at least partically addressed in my previous posts. To just prevent break-thru I just add "DO NOT BREAK THRU" on the hole callout.

Also look at my 3 Jun 08 17:30 post.

KENAT, probably the least qualified checker you'll ever meet...

 

[ewh]

I agree with KENAT. If there is more to the issue, such as limited space, I would consider calling out the pilot diameter as reference and its depth with any required tolerances. If you are extremely limited on available space, you could also specify FLAT BOTTOM.

Believe it if you need it or leave it if you dare. - [small]Robert Hunter[/small]

 

[KimBellingrath]

That's a good question about the word 'drill'. I have always used the term "DRILL POINT" to describe the deepest part of the tap drill hole. The second method used if it's important to control the drill point depth is to use a cross section and in the hole callout just state "TO DEPTH SHOWN IN SECTION A-A" then dimension it there.
A third way often used when working on castings is to control the minimum wall thickness created by any machining operation in a general note. This keeps you from breaking through and controls how deep you can drill for threads - mostly used when castings are used in vacuum environments. Just follow up with minimum thread depths on your callouts.

My favorite is "DO NOT BREAK THRU" short and sweet, no?

 

[ewh]

Yes, a section view is a good solution.

Believe it if you need it or leave it if you dare. - [small]Robert Hunter[/small]

 

[KENAT]

Yeah, for more complex situations a section's often good as after all, a picture paints a thousand words.

I'll always go out of my way to avoid any terms like drill or drill point etc. Not just because of 1.4(e) but also because I had it hammered into me when I started out and I still flinch about it;-).

KENAT, probably the least qualified checker you'll ever meet...

 

[btrueblood]

"Now if we extend the tap drill beyond the threaded hole we will normally define that dia but often we deliberately choose a smaller dia than either the tap drill or thread minor dia to avoid confusion (arguably at the expense of an extra machining step). "

But, if I wanted to use the maximum possible hole size (in my case, in a particular drawing, because it forms a flow passage), and that max. hole size is the tap drill size, is there something that forbids me from calling out the hole dimension (and, yes, I agree, and the hole is called out in a seperate section view)? Maybe as long as I don't say "drill", and just show the dimension line to the point of the hole.

I guess, once again, I take exception to a specification that forces "the expense of an extra machining step".

sign me: Ben "Rebel without a clause" Trueblood

 

[KENAT]

We will sometimes just use the recomended tap drill dia, like you say it saves a machining step and increases dia. The using a smaller dia is kind of lame, can't remember the details now though, been on vacation since.

If the diameter of the 'continuation' hole matters it should be dimensioned, and this will match the dim of the tap drill. However, you're only dimensioning the portion of the hole left after the thread is cut, you're not explicitly defining the tap drill, just matching the expected value. Or something like that.

I don't see that the standard is forcing an extra machining step, more likely me (or relevant engineer) being a dumb A$$ that particular day.

KENAT, probably the least qualified checker you'll ever meet...

 

[btrueblood]

Fair enough. I think the real issue is the use of terms such as "TAP" or "DRILL", and will keep trying to eliminate these as I go along.

 

[KENAT]

If only I'd used the search tool more dilligently.

thread1103-156220

KENAT, probably the least qualified checker you'll ever meet...

 

[kbro151]

Regarding specifying the tap drill size on a drawing, the issue of formed threads was not mentioned. From my experience, TAP usu. refers to cutting threads, but I believe it can encompass forming. If you specifically want threads either cut or formed, then you should specify, either by stating that explicitly on the face of the drawing or calling out a drill size.