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ArnaudGOELZER14-Alexandrite
14-Alexandrite
February 21, 2022
Solved

Help for creating an annotation, driven dimension on diameter

  • February 21, 2022
  • 1 reply
  • 12135 views

Hello,

 

I would like to know how can I create a dimension driven (annotation) on a diameter whose annotation plane is parallel and passing through the axis of revolution?

 

This is what i can currently do with creo 7:

 

I can show dimension from revolution sketch [see dim 1 in the print screen1] : orientation is ok => I want to reproduce the same result with a dimension driven via annotation menu 

 

If i create annotation dimension on the front annotation plane by selecting face of the cylinder, creo desn't want to proceed. I can only select edges of the cylinder but creo see that dim like a linear dim (not diameter). So orientation is ok [see dim 2 in the print screen1].

if I add a flat on the cylinder, the driven dim disappears and it is impossible to show it or re-create this dimension because of the flat. [see print screen2]  => that's why i don't want to use this way.


If i really want to create a dimension by selecting the face (not edges) of the cylinder, first I have to use the top annotation plane and the annotation is created like diameter driven dimension [see dim 3 in the print screen1]. But orientation of the diameter is not the one i want and it's impossible to change it corresponding of front plane.

 

Can you help me find a way to create the annotation I need?

Regards,

Arnaud

Best answer by sacquarone

Hello @pausob 

 

This is a very good question, and complicates significantly the investigation of this given use case. In few words:

  • This occurs because all parent references are lost for the impacted Annotation Element in such situations
  • No other choice therefore to:
    1. Create new references (if not available in geometry, like in this use case)
    2. Redefine parent references of the impacted Annotation Element afterwards

 

I registered for you a little movie reproducing the issue first, and then providing guidance on "how to resolve" in similar situations.

 

Hope this helps,

 

Regards,

 

Serge

 

(view in My Videos)

1 reply

P
19-Tanzanite
pausob19-Tanzanite
19-Tanzanite
February 22, 2022

I'm not totally sure why you want to make a driven dimension when you can simply show the driving dimension in an annotation state, but one way is to make your sketch of the cross-section of revolution "external" and then annotate this sketch.  You'll need an extra datum point in it so that you can dimension the diameter by making a linear dimension between this point and the "edge" of the cylinder (the vertical line in the sketch), and you'll have to add the Ø symbol by editing the dimension text: 

pausob_0-1645519241463.png

Then after creating flats, etc.., your driven dimension will not fail because it's not tied to any solid geometry:

pausob_1-1645519601651.png

 

A
ArnaudGOELZER14-AlexandriteAuthor
14-Alexandrite
February 23, 2022

Thanks for you're reply,

 

I prefer not create a sketch dedicated to dimensioning. I have to doing all the dimensioning work with the annotation menu (or via an annotation function)
I add in this post a second example which shows that it's not possible to reuse the sketch of the revolve function. Please see print screen [revolution1] + [relovution2]
Here we have an inherited part in which we created an offset in order to remove material everywhere in a function (which is useful for complex parts).
If we display the dimensions of the inherited part, it is not correct because it dosen't take into account the offset . It is therefore necessary to go through annotations to be able to set the dimensions of the part after offset.
It is in this kind of case where I cannot reorient my dimensions on the parallel plane of the axis of revolution

P
19-Tanzanite
pausob19-Tanzanite
19-Tanzanite
February 24, 2022

Yes, I see the difficulty in trying to dimension cylindrical surfaces on the annotation plane that their axis of revolution lies upon...  I don't know the trick.

Instead of sketches, you can attach datum points to the surfaces and dimension to these "construction" points...

Or maybe you could make a cross-section and use its lines to construct the annotation dimension...  You can turn off the hatching to make it look better:

pausob_0-1645666913633.png

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