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]

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).

 

[MikeHalloran]

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

 

[KENAT]

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 him;-).

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

 

[fcsuper]

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

 

[MikeHalloran]

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

 

[ewh]

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. - [small]Robert Hunter[/small]

 

[KENAT]

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...

 

[CheckerRon]

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

 

[KENAT]

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...

 

[MadMango]

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 to make the best use of Eng-Tips Forums?

 

[KENAT]

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...

 

[MadMango]

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 to make the best use of Eng-Tips Forums?

 

[drawoh]

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

 

[MikeHalloran]

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

 

[KENAT]

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 ;-)

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...

 

[pierdesign]

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.

 

[btrueblood]

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.

 

[KENAT]

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...

 

[WHITMIREGT]

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.