×
INTELLIGENT WORK FORUMS
FOR ENGINEERING PROFESSIONALS

Log In

Come Join Us!

Are you an
Engineering professional?
Join Eng-Tips Forums!
  • Talk With Other Members
  • Be Notified Of Responses
    To Your Posts
  • Keyword Search
  • One-Click Access To Your
    Favorite Forums
  • Automated Signatures
    On Your Posts
  • Best Of All, It's Free!
  • Students Click Here

*Eng-Tips's functionality depends on members receiving e-mail. By joining you are opting in to receive e-mail.

Posting Guidelines

Promoting, selling, recruiting, coursework and thesis posting is forbidden.

Students Click Here

Jobs

Thread Depth Specifying - Sanity Check Requested
3

Thread Depth Specifying - Sanity Check Requested

Thread Depth Specifying - Sanity Check Requested

(OP)
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...

RE: Thread Depth Specifying - Sanity Check Requested

I use the min callouts also, unless a specific function requires a max. thread depth control also (rare).  But, I can also break the link between hole precision (dec. pts.) and depth precision pretty easily, and will sometimes go that route (e.g. control depth +/- .03 to .06).

RE: Thread Depth Specifying - Sanity Check Requested

Thru to a cross hole is ambiguous because of the cross hole's diameter.  Sometimes you want to go halfway, sometimes not.

I have on occasion had to call out a specific number of thread turns with a tolerance range, something you can do, and occasionally must do, on a screw machine.  It should be a flag for the next re-design, of course.

"It takes up too much room on the drawing" and "We don't inspect that anyway" should be firing offenses, imho.  They are indications that someone may not have his head screwed on straight.



 

Mike Halloran
Pembroke Pines, FL, USA

RE: Thread Depth Specifying - Sanity Check Requested

(OP)
Mike, so what do you do in that case where you want to intersect a thru hole?  

I probably should have said that I normally show a cross section, which arguably obviates the need to say anying about depth.  Also I suppose the note as worded only works if the hole from the face to the other hole is of smaller dia than the hole you're intersecting, as was the case on this drawing.  Given this I dont' see that what I put is ambiguous.  Do you mean it needs a qualifier like 'TO FULL DIA" or something?

Firing offence, more likely I'll get fired for upsetting himwinky smile.

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

RE: Thread Depth Specifying - Sanity Check Requested

I don't see what the issue is either way.  It does seem redundant to me to even have "full thread" in your callout.  If the end condition doesn't matter, just call out the min.

Another piece on info I don't add is the drill size, since this is already an integral part of the thread spec.

Matt Lorono
CAD Engineer/ECN Analyst
Silicon Valley, CA
Lorono's SolidWorks Resources
Co-moderator of Solidworks Yahoo! Group
and Mechnical.Engineering Yahoo! Group

RE: Thread Depth Specifying - Sanity Check Requested

I'd be inclined to give a dimensioned depth for the smaller hole, as if the cross hole were not present, because you don't know the order in which the two holes will be drilled... and because any other way leaves some ambiguity.

 

Mike Halloran
Pembroke Pines, FL, USA

RE: Thread Depth Specifying - Sanity Check Requested

I agree with Mike in regards to cross holes.  When I was working with servovalves, cross holes were very common.  We always dimensioned the depth, even if it was shown in a section.  We had to have full diameter intersections, and any excess depth would cause flow and/or debris problems, so they had to be toleranced accordingly.

Believe it if you need it or leave it if you dare. - Robert Hunter
 

RE: Thread Depth Specifying - Sanity Check Requested

(OP)
fcsuper, the "full thread" is because otherwise some people will interpret the depth as the depth of the tap hole/total depth.  So either you end up paying extra for a bottom tap or you lose a few threads at the bottom of the hole.  The latter wouldn't obviously comply with the drawing but the former would, while unintentionally costing you money.  Basically giving the machinist freedom to tap drill how far they see fit, the qualifier is used when thru would affect function of the part.  I didn't invent it but it makes sense to me.

Mike & ewh, how did you inspect the depth dimension if it was no longer there on the finished part?  I've been taught that basically you don't give a defining dimension for a feature (bottom of the hole) that isn't there on the finished part.  I could see maybe giving a ref dim that corresponds to the CL of the hole you're tapping into (or far enough in to give you a full dia) but surely not a defining dimension?

I've put a sketch showing what I'm talking about on the drilling thru to hole.  (Its not fully ASME compliant drawing so please don't nit pick)  Seems like what I've been doing may not be best practice so I'm interested to learn otherwise.

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

RE: Thread Depth Specifying - Sanity Check Requested

At my present place we design some complicated manifolds that have bores breaking into or through each other often at single or compound angles. We always specify the depth of each bore, and control the depth tolerance such that it gives us at least a 50% penetration with the mating bore. The fact that we get the full or greater penetration (which we also show by sectional views) is the inspectable requirement. This, as Mike says, doesn't dictate drilling order.
MIN FULL THD means just what it says. Regarding internal threads, it states that imperfect or incomplete threads generated by the tap do not count in the total specified thread length, block drawing tolerance does not apply, and a pitch or two extra is OK on a blind hole if break through is not a problem. It is a good callout that is a recommended standard where I am now when control is not critical  

RE: Thread Depth Specifying - Sanity Check Requested

(OP)
So if I understand right at least 3 separate posters are saying that I should give a depth for the (.125 in example) hole which intersects the other (.250 in example) hole.  

The depth given would vary by function but for my example might be to the nominal center of the .250 hole.  

The inspection dictated to verify the depth is not to check the actual depth but verify a full diameter breakthrough to that depth?

By the way, I don't see how my original call out dictates drilling order, it just means drill to through to where the (in my example .250) hole is or will be.  I don't see that it explicitly says the .250 must be there first.  However I now accept doing it this way doesn't appear to be best/common practice.

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

RE: Thread Depth Specifying - Sanity Check Requested

Quote:

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

Looks like you are dictating order in your above example, as the "other hole" has to exist first.  I've designed my share of hydraulic manifolds, and I always made my call outs to include the diameter and depth of every hole or feature.

For general thread depths I would simply put "<depth symbol>.500 THREADS".  If the features are critical, I would call out:

<dia symbol>.201 <depth symbol>.375
<depth symbol>.250 THREADS

"Art without engineering is dreaming; Engineering without art is calculating."

Have you read FAQ731-376: Eng-Tips.com Forum Policies to make the best use of Eng-Tips Forums?

RE: Thread Depth Specifying - Sanity Check Requested

(OP)
MAD, As I put immediately above I disagree that I'm defining process order.  

Per ASME Y14.5M-1994 I'm defining the end product.  In the end product the smaller hole is thru to the .201 hole.  I don't care what order they're done in so long as they fully intersect.  

However, I now accept that giving a depth for that hole is the standard way and I just changed the drawing which this came up in.

So Mad, you inspect the threads depths for min & max and if the depth tol exceeds the max (for me 3 DP is normally +-.005) you reject the part, even tho in most cases it's probably functional?

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

RE: Thread Depth Specifying - Sanity Check Requested

OK, so perhaps my examples were not the greatest.  For non-critical holes, the depth is designed deeper than the fastener engagement going into it, on the order of 1/2 DP (usually 2 decimal tolerance, +/-.03).  For critical holes, yes, if the threads fall outside the +/-.005, the parts are rejected.  Then QA calls and someone test-fits a fastener to buy-off the parts (works) or  not (doesn't work).  Its not a perfect system.

"Art without engineering is dreaming; Engineering without art is calculating."

Have you read FAQ731-376: Eng-Tips.com Forum Policies to make the best use of Eng-Tips Forums?

RE: Thread Depth Specifying - Sanity Check Requested

KENAT,

   If I specify a thread and a depth, I expect my thread gauge to go down that far.

   On my metric drawings, I make sure my hold depths are to a full metric value, i.e. no decimal places.  This sets the tolerances to +/-1mm as per my drawing notes.  I figure this is sloppy enough.

   Sometimes I add a note stating that tapped holes are to be blind.  

   If my requirement is any more complicated than that, I add a section view to the drawing, and apply dimensions accordingly.

                        JHG

RE: Thread Depth Specifying - Sanity Check Requested

One good reason for specifying the depth of a hole that is later removed or that intersects a pre-existing hole, and is in either case not inspectable in the finished part, is that the CNC machine that does the drilling needs to have the tool set to a specific position, whether it's cutting air or not at the end of the drill cycle.

Similarly, you need to have benchmarks for in-process checking, when the hole  bottom _may_ exist.

You just don't want to get into an argument with a machine driver about what 'intersect' means... because even if you 'win' the argument, you'll be having it again the next week with the next machine driver.



 

Mike Halloran
Pembroke Pines, FL, USA

RE: Thread Depth Specifying - Sanity Check Requested

(OP)
Hmm, so one post I'm lambasted for supposedly dictating how a part is made and then another I'm told that a benefit of the way it should be done is telling them how to make it.

Signed,

Confused of Santa Barbara winky smile

Anyway, thanks all.  

I'm changing how I expect hole intersections to be dimensioned to match the consensus here.  

While there are a few disenters I'm still of the opinion that usually giving 'min full thread' is a good option, perhaps better than the other obvious options (especially taking into account my CAD systems limitations, as much as I hate to let that drive what I do).

 

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

RE: Thread Depth Specifying - Sanity Check Requested

In these situations it is beneficial to consider dimensioning schemes from the NC programmer / machinists perspective.  As other poster stated, the machine needs to have a depth dimension whether or not that hole depth becomes imaginary at inspection.  It's the same for thread depths, the machine needs depth programmed depending on tap and tap head used.

On a semi-related note on thread depths: recently I've seen twice now vertical mills and tooling that cuts internal threads via circle interpolation using an incredibly small barb insert cutter, like a miniature boring bar.  Effect is full thread to hole bottom.

RE: Thread Depth Specifying - Sanity Check Requested

Boy, I don't agree with a fictitious hole bottom, but only because I had bad experiences with that scheme.  "THRU NEAR SIDE" is preferrable, with "fully threaded" equally descriptive if necessary (my opinion only, and I can see the justification for thread depth callouts).  But, as a young dumb fresh grad, I had parts rejected repeatedly by a QC engineer because the holes didn't meet the minimum thread depth (because there was no material left inside the cross hole to be threaded, there were no threads in the empty space, therefore the parts were rejected).  Back and forth I would go between the design engr, who just didn't want to change the print to satisfy some snotty tech, and the inspector...ad nauseum...until we finally agreed to specify the whole thing with a very verbose note (ok, there was more going on at the hole intersection than just a thread, too).  

The idea that a view showing a hole intersecting only one side of the cross hole could be mis-interpreted as going thru both sides of the hole violates the 1st principles of drawings (features not shown on the print aren't allowed).  

Mike says "You just don't want to get into an argument with a machine driver about what 'intersect' means... because even if you 'win' the argument, you'll be having it again the next week with the next machine driver."

But, I'd rather argue with a machine driver than an inspector.

RE: Thread Depth Specifying - Sanity Check Requested

(OP)
I'd been led to believe that when defining dimensions & tolerances on a part you did so in the following order of precedence:

1.  Dimension to support function - make sure that a part made to print will work as required.

2.  Dimension to support inspection - make sure that inspection can verify that the part meets the requirements that allow it to function correctly i.e. is built to print.

3.  Dimension to support manufacture - if it doesn't conflict with 1 & 2 above dimension in a way that simplifies manufacture of the part.

Am I wrong, or perhaps in the ever more closely integrated CAD/CAM world this has changed?
 

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

RE: Thread Depth Specifying - Sanity Check Requested

First of all, we must be able to read a drawing, not interpret a drawing.

If the cross hole is larger than the threaded hole, I would state after the thread callout " MAJOR DIA OF THREAD MUST BREAK THRU" This is easy to check by threading in a screw or bolt.

If the cross hole is smaller than the threaded hole, call out a depth on the threaded hole.

RE: Thread Depth Specifying - Sanity Check Requested

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.

RE: Thread Depth Specifying - Sanity Check Requested

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.

RE: Thread Depth Specifying - Sanity Check Requested

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. - Robert Hunter
 

RE: Thread Depth Specifying - Sanity Check Requested

(OP)
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...

RE: Thread Depth Specifying - Sanity Check Requested

(OP)
"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...

RE: Thread Depth Specifying - Sanity Check Requested

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.

RE: Thread Depth Specifying - Sanity Check Requested

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. - Robert Hunter
 

RE: Thread Depth Specifying - Sanity Check Requested

(OP)
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 aintwinky smile.

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

RE: Thread Depth Specifying - Sanity Check Requested

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?

RE: Thread Depth Specifying - Sanity Check Requested

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...

RE: Thread Depth Specifying - Sanity Check Requested

(OP)
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...

RE: Thread Depth Specifying - Sanity Check Requested

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. - Robert Hunter
 

RE: Thread Depth Specifying - Sanity Check Requested

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?

RE: Thread Depth Specifying - Sanity Check Requested

Yes, a section view is a good solution.

Believe it if you need it or leave it if you dare. - Robert Hunter
 

RE: Thread Depth Specifying - Sanity Check Requested

(OP)
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 itwinky smile.

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

RE: Thread Depth Specifying - Sanity Check Requested

"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

RE: Thread Depth Specifying - Sanity Check Requested

(OP)
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...

RE: Thread Depth Specifying - Sanity Check Requested

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.

RE: Thread Depth Specifying - Sanity Check Requested

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

thread1103-156220: Thru To Bore Note

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

RE: Thread Depth Specifying - Sanity Check Requested

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.

RE: Thread Depth Specifying - Sanity Check Requested

(OP)
kbro, this is covered by ASME Y14.5M-1994 1.4e "However, in those instances where manufacturing, processing, quality assurance, or environmental information is essential to the definition of engineering requirements, it shall be specified on the drawings or in a document referenced on the drawing."

KENAT,

Have you reminded yourself of FAQ731-376: Eng-Tips.com Forum Policies recently, or taken a look at posting policies: http://eng-tips.com/market.cfm?

RE: Thread Depth Specifying - Sanity Check Requested

kbro,

I agree with KENAT's statement, however I have a comment for you.  Why would you specify roll vs. cut?  The end result is the same.  Let the vendor work it out as to which method is best.  I can imagine scenarios where roll is a much, but these are extremely rare in my opinion.  

In either case, do not callout the drill size.  Simply call out the thread spec.  If you need to mention the process, then do so (without the drill size).  The final ID of the thread is already specified by the thread callout itself.

Matt Lorono
CAD Engineer/ECN Analyst
Silicon Valley, CA
Lorono's SolidWorks Resources
Co-moderator of Solidworks Yahoo! Group
and Mechnical.Engineering Yahoo! Group

RE: Thread Depth Specifying - Sanity Check Requested

(OP)
Just re-read kbro post and I agree with Fcsuper that while you may use different tap sizes based on process that probably isn't what you should specify on the drawing.  You should explicitly specify 'rolled' or 'cut' if you require it.  

I know there are situations where rolled are (were?) preferable to cut threads.

KENAT,

Have you reminded yourself of FAQ731-376: Eng-Tips.com Forum Policies recently, or taken a look at posting policies: http://eng-tips.com/market.cfm?

Red Flag This Post

Please let us know here why this post is inappropriate. Reasons such as off-topic, duplicates, flames, illegal, vulgar, or students posting their homework.

Red Flag Submitted

Thank you for helping keep Eng-Tips Forums free from inappropriate posts.
The Eng-Tips staff will check this out and take appropriate action.

Reply To This Thread

Posting in the Eng-Tips forums is a member-only feature.

Click Here to join Eng-Tips and talk with other members!


Resources