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How can you dimension nearly parallel lines in a drawing?

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How can you dimension nearly parallel lines in a drawing?

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

1 ACCEPTED SOLUTION

Accepted Solutions

Re: How can you dimension nearly parallel lines in a drawing?

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

7 REPLIES 7

Re: How can you dimension nearly parallel lines in a drawing?

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.

Stephen Williams
Pro/E Version 15/16 (Circa 1995/1996)

Re: How can you dimension nearly parallel lines in a drawing?

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

Re: How can you dimension nearly parallel lines in a drawing?

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?

Re: How can you dimension nearly parallel lines in a drawing?

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).

Re: How can you dimension nearly parallel lines in a drawing?

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.

Re: How can you dimension nearly parallel lines in a drawing?

My mistake, I was looking in the options for drawing properties. Anyhow, it worked; this is exactly what I was looking for (if only I tried this 3 hours ago). Thank you so much!

Re: How can you dimension nearly parallel lines in a drawing?

To dimension small angles, place the following in your config.pro:

!The following for ease in placing small angular dimensions

comp_angle_offset_eps 91

comp_normal_offset_eps -1

This may be what you are looking for.