Results 1 to 5 of 5

Thread: GD&T on a dovetail feature

  1. #1
    Associate Engineer
    Join Date
    Dec 2017
    Posts
    2

    Question GD&T on a dovetail feature

    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.

    Attached Images Attached Images

  2. #2
    Technical Fellow jboggs's Avatar
    Join Date
    Mar 2011
    Location
    Myrtle Beach, SC
    Posts
    749
    Curious to see how the experts answer this one.

  3. #3
    Administrator Kelly Bramble's Avatar
    Join Date
    Feb 2011
    Location
    Bold Springs, GA
    Posts
    2,094
    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.
    Tell me and I forget. Teach me and I remember. Involve me and I learn.

  4. #4
    Associate Engineer
    Join Date
    Dec 2017
    Posts
    2
    Quote Originally Posted by Kelly Bramble View Post
    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.

    Quote Originally Posted by Kelly Bramble View Post
    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.

    Quote Originally Posted by Kelly Bramble View Post
    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.

  5. #5
    Administrator Kelly Bramble's Avatar
    Join Date
    Feb 2011
    Location
    Bold Springs, GA
    Posts
    2,094
    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.
    Tell me and I forget. Teach me and I remember. Involve me and I learn.

Posting Permissions

  • You may not post new threads
  • You may not post replies
  • You may not post attachments
  • You may not edit your posts
  •