Combining Dimensions

[solidhardhead]

Is it possible in a Solidworks drawing to combine dimensions into one leader line? For example:

1.25" DIA. HOLES ON A 25" BOLT CIRCLE

In this case the "hole dia" and the "bolt circle" dimension would automatically update as the model changes.
Yet they both fall under the same leader line.

Thanks

 

[TheTick]

I do this using custom properties. I incorporate the dimensions into a custom property, then use the custom property in a note.

 

[handleman]

There's not any way to link text in one dimension to a value of another. If you really want to force this, you have a couple of options.

Assuming that you have a hole callout type dimension (Ø1.25") on a leader, you can create a leaderless note with the text "HOLES ON A BOLT CIRCLE", put your cursor between "A" and "CIRCLE", and click the actual dimension for Ø25". You can then hide (not delete) the Ø25" dimension, and the value will be linked into the note. Position the note where you want it in relation to the hole callout, select both, right click, and choose "Group". Note that "Group" will only be available if the note belongs to the view. If you create the note too far away from the view then it will belong to the sheet rather than the view. If this happens, just change the leaderless note to one with a leader and drag the leader to some geometry on the view. You can then switch back to no leader and the note will stay with the view. This method is also your only option if the dimension has to be a linear type dimension (witness lines, arrows, etc.) rather than a hole callout type dimension.

The other way would be to create both dimensions, add one note with a leader, link both values into that note, and hide the original dims.

I wouldn't want to do either of these 50 times a day, but if you just need to do a couple then this will work.

Custom properties will work as well, but they do require some additional setup in the part file.

 

[nsessions]

This is WONDERFUL!
how do you show a dimension once you have hidden it?
Cheers Nick

 

[SolidAir]

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SA