General profile governing limits

[decS]

I have a quandary that appears quite often on prints I work with.

A given part has a general profile to govern undimensioned features. On said part I have a blind, threaded hole called out on the print to Y14.6 standards. There is a section view of this hole with a cylinder depth called out However a drill tip is modeled with the part. This drill tip is not specifically defined on the print. Does the general profile apply to the cone formed by the modeled drill tip?

I would like to argue that it does not apply as the drill tip geometry would then require that a drill be used to form the hole rather than some other machining process. Especially when this drill tip is likely automatically modeled by a hole wizard in the designer’s CAD program.
A further slippery slope, do I need my CMM to construct a cone for the drill tip to ensure that the profile is met at the base of the hole?

 

[greenimi]

How the general profile is callout on your drawing? Could you, please post that section of the drawing where the general profile is indicated?

 

[Doug Hunter]

Hi DecS,

I second Greenimi. However, I will offer this also: Assuming that the part has a 3-D model, and the 2-D drawing is aligned with the 3-D model, then the general profile tolerance would apply to the 3-D geometry, even when there is no basic dimension provided. The 3-D model is usually assumed to be nominal (it's better to have a general drawing note that states this specifically).

 

[greenimi]

Assuming that the part has a 3-D model, and the 2-D drawing is aligned with the 3-D model, then the general profile tolerance would apply to the 3-D geometry, even when there is no basic dimension provided. The 3-D model is usually assumed to be nominal (it's better to have a general drawing note that states this specifically).

So, how to you know when apply general profile and when not?

 

[decS]

The note would go something like this:

“This is a minimal dimension drawing. The CAD model is the master for all dimensions not shown on the drawing. Part profile 0.025 A B C unless otherwise stated”

I’ve also attached an example of one of the points in question.

 

[greenimi]

Part profile 0.025 A B C unless otherwise stated”

So, is what you are looking for stated otherwise or it is not ?
What exactly you are looking for?

 

[mfgenggear]

OP
I don't believe this is addressed by ASME Y14.5.
My customers specified their own internal specification. As drill points are specified as standard drill points.
Old school it was standard to be option configuration and could be flat bottom or the
Included of a standard drill point.
What was important that the depth is held .
To allow proper tapping for the correct depth.

However the proper procedure should be to contact the design authority, customer
To clarify the configuration and dimension.
Never assume.

 

[Burunduk]

Note that as far as ASME Y14.5 is concerned, the Fundamental Rules require you to specify a tolerance for every single feature of the part. Here is rule (a) from the 2018 edition:
"(a) Each feature shall be toleranced. Tolerances may be
applied directly to size dimensions. Tolerances shall be
applied using feature control frames when feature defini-
tion is basic. Tolerances may also be indicated by a note or
located in a supplementary block of the drawing format.
See ASME Y14.1 and ASME Y14.1M. Those dimensions
specifically identified as reference, maximum,
minimum, or stock (commercial stock size) do not
require the application of a tolerance."

To comply to that you technically need some kind of tolerance even for that conical hole end. The general profile can apply to it, but I guess it wouldn't make sense to inspect or reject the part if a different drill point angle was used and now the surface is non-conforming but there are zero consequences to that. The nice thing about a general profile is that it doesn't form a unique requirement specifically for that surface, so you have more legitimacy to skip it and measure elswhere.

 

[greenimi]

This drill tip is not specifically defined on the print. Does the general profile apply to the cone formed by the modeled drill tip?

I would like to argue that it does not apply as the drill tip geometry would then require that a drill be used to form the hole rather than some other machining process

If you don't have anything specified I WOULD ARGUE what the general profile would apply otherwise the drawing is incomplete.
The purpose of the general profile is to MAKE the drawing complete so if you interpret the drawing YOUR WAY then that's defeting the purpose of the NOTE ( Part profile 0.025 A B C unless otherwise stated”)

 

[Doug Hunter]

So, how to you know when apply general profile and when not?

At my previous employer, we had defined the standard that the (generous) default profile tolerance applied to everything that was not otherwise controlled/specified, and that only an annual layout was required. If more frequent quality control checks are required, then I recommend not leaving it to the default profile tolerance.

 

[greenimi]

The nice thing about a general profile is that it doesn't form a unique requirement specifically for that surface, so you have more legitimacy to skip it and measure elswhere.

Yes, and I am sarcastic here....the nice thing is that UOS has multiple legal interpretations.

 

[Doug Hunter]

The note would go something like this:

“This is a minimal dimension drawing. The CAD model is the master for all dimensions not shown on the drawing. Part profile 0.025 A B C unless otherwise stated”

I’ve also attached an example of one of the points in question.

In that case, I stand by my assessment. You have other options for allowing alternatives, such as drawing notes added to that view.

 

[3DDave]

I have a quandary that appears quite often on prints I work with.

A given part has a general profile to govern undimensioned features. On said part I have a blind, threaded hole called out on the print to Y14.6 standards. There is a section view of this hole with a cylinder depth called out However a drill tip is modeled with the part. This drill tip is not specifically defined on the print. Does the general profile apply to the cone formed by the modeled drill tip?

I would like to argue that it does not apply as the drill tip geometry would then require that a drill be used to form the hole rather than some other machining process. Especially when this drill tip is likely automatically modeled by a hole wizard in the designer’s CAD program.
A further slippery slope, do I need my CMM to construct a cone for the drill tip to ensure that the profile is met at the base of the hole?

This requires the secret handshake. They ignored the problem, you can ignore the problem. This is seen by the way ASME Y14.5 also ignores the problem. The universal answer is the depth to the drill point can be controlled if it is critical and, for threaded holes, the usable full thread. Note that profile tolerance is not applied to the partial threads. Almost always the functional requirement is to have enough hole depth for the cheapest tapping operation to fully thread to the depth required.