Why shouldn't I dimension blind holes to drill tip on drawings?

We have been dimensioning our blind holes from the start surface to the drill point. This is being done at the request of our machine shop. I was told that the reason is, the cnc operators want be be able to compare the depth readout on their cnc's with the value in the drawing note.
Every standard I have seen calls for holes to be dimensioned to their full diameter depth.
Has anyone else dealt with this issue? Should the cnc operators really need the bind holes dimensioned to the drill point? We are going thru our company standards and I would like to know if we should join the 99% of companies that dimension to the full diameter depth or not.
I need a further explaination of the pros and cons of this practice so we can decide which way to go.
Thanks,

Dear miller:
  Quoted Text Here  
Manufacturing engineering (aka. "methods" guys) will produce such a drawing.
  Quoted Text Here  
If the angle on the drill point is absolutely the same every time a hole is drilled, this might work. But with every hole, this point moves away.
I suspect what they are looking for is a way to be sure they do not break through, in a world where the number of steps to yield the final hole precludes doing multiple stages with ever larger bits, followed by a ream to depth for the final pass.
It used to be common for one department to produce drawings for the "inspectors", and another set of drawings for those that make the part. What organization do you have at your place of work? How likely is your management to take your drawing(s) to an outside job shop, and have them produce a load of scrap because they don't taper drill bits like your folks do?
My two cents worth.
David A. Smith

On Mon, 21 Jan 2008 12:58:12 -0800 (PST), miller
  Quoted Text Here  
Interesting question. I can discuss it, though without any great insight. There is a philosophical issue about building quality into a product as opposed to testing/measuring it in.
How does one measure a blind hole? Depth is the prime consideration, evidently: if the test stylus is pointed, then it should probe the deepest point - the center of the hole. How can this be assured? Perhaps only with a near replica of the initial drill. Hence a drill point hole is somewhat hard to measure.
But then, a CNC machinist can set a tool to touch a surface, and can accurately provide some set cutting depth. Hence a drill point hole is somewhat easy to CNC machine to a set depth.
There is a question as to purpose: what is the purpose of a blind hole? to take a screwed thread, to take a register pin? Either of these might give problems for a hole specified to a drill point's depth.
On balance, I lean towards the 'machine in easily', vs 'test in easily' side, and vote with the machinists.
Brian W

  Quoted Text Here  
Dear Miller-
I'll throw in my 2¢ and agree with Brian, Dave. and Harry...
Being a engineer but having worked in mfg, I tend to want to put the burden on the designers (me & the other engineers)
NOT the machinists & the QC people.
Design gets done once (hopefully) plus engineers & designers have erasers (or back space key)
when a part(s) gets made wrong it costs $$'s
I would dimension the part so it can perform all its needed functions if it meets the print AND it's easy on the guy cutting chips.
Yeah, there are standards on how to dimension a hole BUT what really counts is what the hole is supposed to do..............
A blind hole? Seems to me you don't want break through (or does it really matter?) If the feature matters, you've got to control it
Plus maybe you need a minimum full diameter depth
I would cook up a set of dimensions that reflect whats really important.
Give you machinists & inspectors as much tolerance as possible.
If you can live with +/- .010 don't put +/-.005 on the print ....if a part within +/-.030 will function........give the extra tolerance.
I used to argue with the guys who put +/-.003 on the print when +/-. 010 would work.
Their rationale? The machinist would try harder if he saw +/-.003!
I asked if we were paying for the machinist to meet the print or just try to?
cheers Bob

As Bob said. if breakthrough matters, put a max dimension on the tip of the hole. If the depth of the full OD matters dimension that as a min.

  Quoted Text Here  
I appreciate all your comments. We are a small OEM which does most of our machining in-house. We do occasionally farm machining out and have to revisit our prints before we send them out to ensure they are clear and complete. Our in-house cnc programmers do generate a manufacturing drawing with a tool list but do not add bind hole dims. We do our inspection "at assembly". You can tell from my initial post that I lean towards following drawing standards that dimension blind holes to their full diameter depth but considering the feedback I have received here I'll have to reconsider that position.
Thanks,

Dear miller:
  Quoted Text Here  
Which doubles the cost of engineering, a cost that is probably not captured in the cost of farming out the machining.
  Quoted Text Here  
So inspection levels are 100%. How would you measure from the tip of the hole, to the face on the opposite side? How can you know what angle they faced their tool to, on every hole? I was a machining inspector, and I will tell you that I could not do this without using a sophisticated prgram and a validation machine, that reconstucts the bottom taper from multiple bump points on that "cone".
  Quoted Text Here  
You were right, and you are about to make a mistake, IMO. Adding a callout "no breakthrough" should be entirely sufficient. Inspection sufficient to detect a "dimple", without letting the contractor know, should be sufficient to identify a failure. Better still to create rework methods to fix it when it breaks through, and even better still to design away a blind hole entirely.
Pipes with 0.065" thick walls will handle 1000 psi or more without bursting, on large geometries. So you really need to know what you are trying to keep out of the thread area, or what you are trying to keep from diffusing across the remaining material, and design that "web". Maybe it is being made more complex than necessary.
It is really easy to design a part that cannot be made for infinite dollars. And controlling essentially unimportant dimensions is the surest way to reach that goal.
David A. Smith

In article
  Quoted Text Here  
You have an engineering requirement for a full diameter hole to a certain depth because something is going in the hole: a pin, a thread, or something. That diameter to that depth is your engineering requirement and obviously must be dimensioned and inspected. What it takes to get there is NOT an engineering requirement. The drill point and any overdrill are probably irrevelent to your requirement. Why should an irrelevancy be dimensioned? If it's dimensioned it must be inspected, but if it's irrevelent then it's just costing you money without benefit.
In addition, in many cases I've had to design blind holes where the back of the material was fairly close but I did not want break out. In those cases you can either specify a flat bottom drill, or dimension the drill point, because then the drill point IS an engineering requirement, and should be inspected.
1] be aware that different drill profiles exist 2] specify your engineering requirement

I assume you have in house CNC. In that case, every time a "machinist" makes a mistake, you pay for the scrap part. When a part is dimensioned for simplictty there is less chance of error.
At one time my facility decided that all drawings were to be done metric (back in the 70's). Draftsmen were fine with that, they drew in inches, then output the dwgs in metric. BUT, all the machines were in inches, so every machinist had to convert, on the drawing, to make the part. MANY scrap parts.
I have always dimensioned to the place I care about, be it break thru, thread depth, or flat bottom if required.
One ambiguity when dimensioning to the drill point is that even though the included angle is spec'd, some drill points are thinned at the web, and are nearly a sharp point. While trivial at .100" it's a big deal at 1".
I believe that drawings should be dimensioned from planes so the parts can be fabricated and inspected easily.
How to integrate that into company standards? Good luck. Dave
  Quoted Text Here