GD&T on a dovetail feature

[mathias_tabor]

Hello,

Been updating old prints to use GD&T for clarity. I'm not sure how to dimension this dovetail such that the feature is within .001 along its length. See below for old-style dimensioning. I've circled the note I need tolerancing help on.

[jboggs]

Curious to see how the experts answer this one.

[Kelly_Bramble]

There are several ways to define or rethink your apparent requirements.


Double check your functional requirements to ensure that you understand the requirements. The tolerances and size may be too tight, loose or adequate. Most likely they are too tight.


I would consider specifying a gage pin as opposed to a dowel pin. There is a difference in size and tolerance.


The gage pin method is industry standard for measuring standard dovetails.


Option 1 - Define the horizontal surface 2X as Datum A. Then use a profile of surface tolerance tight enough to achieve your 60 deg. surface orientation and size.


Option 2: Define a Datum Target Line on the tangent edge of one of the gage pins. Then specify a Parallelism of .001 relative to datum A. You should review the angle tolerance on the 60 deg angles to see they are adequate.


Option 3: Simply tighten up the limits of size from 3.435 - 3.430 too maybe 3.435 - 3.434. Rule #1 (Envelope Principle ASME). This reduces the over variability and creates a tight parallelism. But, it reduces to total variability of size. Again, review the angle tolerance on the 60 deg angles to see they are adequate.


Option 4: Review the function and fit requirement and see if you can drop the "Parallel within .001" requirement. and let the simple limit tolerances do the controls. The Parallel specification is unlikely to improve tracking of the dovetail feature.

[mathias_tabor]

There are several ways to define or rethink your apparent requirements.

Double check your functional requirements to ensure that you understand the requirements. The tolerances and size may be too tight, loose or adequate. Most likely they are too tight.

It is my understanding that the current .001 parellelism requirement came about due to the mating part being either too loose or binding along the dovetail length once its gib was adjusted.

I would consider specifying a gage pin as opposed to a dowel pin. There is a difference in size and tolerance.

The gage pin method is industry standard for measuring standard dovetails.

Thank you for the suggestion; I will.

Option 1 - Define the horizontal surface 2X as Datum A. Then use a profile of surface tolerance tight enough to achieve your 60 deg. surface orientation and size.


Option 2: Define a Datum Target Line on the tangent edge of one of the gage pins. Then specify a Parallelism of .001 relative to datum A. You should review the angle tolerance on the 60 deg angles to see they are adequate.


Option 3: Simply tighten up the limits of size from 3.435 - 3.430 too maybe 3.435 - 3.434. Rule #1 (Envelope Principle ASME). This reduces the over variability and creates a tight parallelism. But, it reduces to total variability of size. Again, review the angle tolerance on the 60 deg angles to see they are adequate.


Option 4: Review the function and fit requirement and see if you can drop the "Parallel within .001" requirement. and let the simple limit tolerances do the controls. The Parallel specification is unlikely to improve tracking of the dovetail feature.

I think Options 1 or 4 would work best; basically I'm looking for a way to specify that the total variability of the 3.435/3.430 dimension is less than or equal to .001 over the length of the dovetail. In other words, the dimension is between the limits but doesn't vary more than .001 over the dovetail.

I believe Option 3 would increase the cost too much.

[Kelly_Bramble]

It is my understanding that the current .001 parellelism requirement came about due to the mating part being either too loose or binding along the dovetail length once its gib was adjusted.

Parallelism is a refinement of size. The paralelism tolerance boundaries specified must always be contained within the tolerance boundaries defined by the limits of size - this is Rile #1 in ASME/ANSI standard.

Therefore, if the mating parts were binding it is most likely that the build was out of tolerance or the size limits are not correct for clearance.