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A
aderosa1-Visitor
1-Visitor
March 6, 2017
Solved

How can you dimension nearly parallel lines in a drawing?

  • March 6, 2017
  • 2 replies
  • 5458 views

Hi,

 

I'm working with Creo Parametrics 2.0, and I'm having the most difficult time trying to add a few dimensions to my drawing. I have a tube-like part with a slight draft on the inside of the tube. I want to add an angular dimension from the center line to the inside surface in a section view. The two lines don't intersect and the angle is so small (about a quarter of a degree) that I can't dimension it. I've tried everything but the best I can do is fudge the dimension by making a sketch entity at a reasonable angle, dimensioning it, and moving it to overlap the inner surface. It looks fine, but I know it won't update with the part geometry. The revolve that made this angle was not dimensioned in such a way that model annotations comes up with the right dimension, but I've tried redimensioning it with that angle in mind, and it still won't work. If anyone has any ideas, please let me know!

 

Thanks,

Alex

Best answer by mender

For the desired behavior without needing to temporarily fudge the model, set the config option 'minimum_angle_dimension' to a small value (in degrees).

2 replies

S
23-Emerald III
StephenW23-Emerald III
23-Emerald III
March 6, 2017

Temporarily change the model so it has a larger angle that is easily dimensioned. Then change the dimension to the smaller # you really need.

Then you can show the angle dimension in the drawing.

A
aderosa1-VisitorAuthor
1-Visitor
March 6, 2017

I may resort to that, but I'd like to avoid it if possible. The revolve that caused this problem was dimensioned via the vertices on this part of the draft so the angle itself is hard to capture. Of course I could get it accurate to multiple decimal places, but I'd rather leave the part's design intent intact if I can (I am not the original creator).

M
mender12-AmethystAnswer
12-Amethyst
March 6, 2017

For the desired behavior without needing to temporarily fudge the model, set the config option 'minimum_angle_dimension' to a small value (in degrees).

    A
    aderosa1-VisitorAuthor
    1-Visitor
    March 6, 2017

    That sounds wonderful except I can't seem to find that option in the options tab. Is it perhaps under a different name for Creo Parametrics 2.0?

    M
    mender12-Amethyst
    12-Amethyst
    March 6, 2017

    It's from WF1, so it should work.  In Creo 2, File>Options>Configuration Editor>Add..., Open name 'minimum_angle_dimension' (it'll autocomplete after 'mini'), could use the Find button in the Cfg Editor dialog if you like.

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