Reference a model dimension in a text note?

[curiousmechanical]

Hello Everyone.

I use both SolidWorks 2006 and PRO/E wildfire 2.0 for CAD.

Main Question:

How do I reference a model dimension while making a drawing in Solidworks?


In PRO/E, I would simply write something like "...drill &d45 dia. holes as shown..." Where "&" symbol is used along with the model dimension name d**, to display the actual value of the dimension in the text. Can you do anything like this in SolidWorks? If so, how? I feel like there has to be a way!

Thanks!

 

[handleman]

Sure. While typing the text of the note, just click on a dimension and the text will be inserted.

 

[curiousmechanical]

Thank you for the tip! The trick did work for notes. Although, it doesn't work for following case:

Say I am creating a c'bored tapped thru hole...I will use the whole wizard to call out the tapped thru hole. Then, I would like to add c'bore information (depth and diameter) to the hole wizard's callout. I don't want to have a seperate callout for each feature. Therefore, I am trying to figure out the nomenclature needed to reference those dimensions.

 

[SolidAir]

curiousmechanical,

Goto Insert, Annotations, Hole Callout. Select the counterbored hole and see if the result is what you want.

SA

 

[CorBlimeyLimey]

curiousmechanical ... submit an ER if you need the counterbored tapped hole callout often.

 

[handleman]

You can't link text in one dimension to the value of another dimension. If I'm remembering right, a SolidWorks hole callout is actually a form of dimension rather than a note. As such, I don't think you can link text in a true hole callout to another dimension.

If you want your note to be linked to a dimension but not have that actual dimension show you can RMB on the dimension and choose "Hide" after linking.

There is an option somewhere under Tools->Options that mentions something about viewing linked text while editing a note. That option controls whether the linked value or the actual syntax is displayed during editing of the note. I'll check it tomorrow unless someone beats me to it...

 

[handleman]

I found it. It's not in Tools->Options. It's under the View menu. Make sure that View->Annotation Link Variables is checked. That will allow you to see the syntax for linking dimension values to a note.

 

[curiousmechanical]

handleman,

Thank you very much!

The syntax was exactly what I was looking for, [example: "RD1@Drawing View2"]. Although, I am very dissapointed to find out that I cannot reference another dimension within a dimension using this syntax. Example: I tried, [<DIM> check out "RD1@Drawing View2"]. The syntax did not reference the dimension. The result was simply, [.250 check out "RD1@Drawing View2"].

Thank you for saving me more hours of trying to figure it out!