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Pro/Engineer   May 2000   Tip-of-the-Month

When "Show Dims" Won't Work Right

What do you do when a dimensions needed on a drawing won't "Show" correctly in the view or orientation desired in the drawing?  Even when the model contains the dimension you need to display, sometimes Pro/E won't "Show" it as you would like to see it.

Sometimes the problem is in the sketch orientation, sometimes in the view position, but other times it's just Pro/E being ornery.  Rounds are a classic for this very annoying behavior.

Here are a few things to work with in correcting a dimensioning display problem.

First, try to figure out why the dimension won't show as you think it should.  If it's because of a view or sketch orientation, can it be fixed by showing the drawing view slightly different?  Also, try showing the dimension in one view then use Detail > Switch View to move it to another.

Second, can the dimension be "forced" to behave correctly by using Mod Attach?  This often works for rounds.  Simply select Detail > Mod Attach then the dimension.  Possible places for attaching the leader will highlight in magenta.  See Figure 1.

May 2000 Fig.1 May 2000 Fig.2
Figure 1
Figure 2
(Note:  This can be extremely useful when multiple rounds are created in one feature.  With Mod Attach you can move the dimension to another part of the round like in Figure 2.)

Third, Create the dimension.  PTC purists often look at created dimensions as bad, bad.  (I'm not sure they have any real world experience anyway.)  If you took the Introduction to Drawing course by PTC you know how they preach against the Create Dimension functionality.  Yet, sometimes it is just the ticket, but we recommend you use it sparingly.

Fourth, depending on the situation, another way to display a dimension is in a note.  To do this, identify the dimension name (Pro/E defaults look something like d34 or d34:4) then put it in the note text with an "&" in front like &d34.  This will show the dimension in the note.
May 2000 Fig.3
Figure 3
May 2000 Fig.4
Figure 4

This technique using an "&" can also be used to add more dimensions to an existing one like in Figure 3.  In this case, the text used for the note is:

{0:&p8}{1:X }{2: n }{3:@D}{4: THRU}
{5:ON }{6: n }{7:&d3}{8: BC}

The text is shown in the note with Switch Dims in Figure 4.  (In the text above, the @D is the original dimension, the rest is added using Modify > Modify Text > Full Note.  The :12 after each dimension name is assembly information.)

I have heard it said that you can plant a model dimension within a created dimension by replacing the @D with something like @O&d34.  I use this technique a lot for putting text in a dimension form (like @O NO PAINT THIS AREA), but I have not been able to make this work for dimension values.  It works great for text, but not for values.  If you know this trick, please tell us.  We'll publish it here with your name.

Thank you to Izaak Koller and Santo Uccello of Hunter Industries, San Marcos, CA for suggesting this Tip-of-the-Month.

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