If you create drawings like myself, you will almost exclusively use the Insert à Model Items (Fig 14-0) to populate your drawings.  The problem with this way of dimensioning is that drastic changes during an ECO, EO, ect. model my cause you to want to delete dimensions from sketchs if you don't know the new value before another dimension is changed.

Fig 14-0

For example, a request for change "(EO, ECR, ECO, DCN ...)" of a drawing that has been created using Insert à Model Items (Fig 14-0).

A driving angle dimension in sketch of the model, to reference dimension and add the height and width dimensions of the angle to the drawing instead.  (Remember you have used Insert à Model Items to make the drawing.)

 

This tip we will discuss the changing of a drawing that uses the Insert à Model Items (Fig 14-0) way of creating a drawing.

Fig 14-1

 In order to make this examples change, do as listed below which causes more work on their part.  

• Open the part model that created the drawing.
• Edit the sketch the angle dimension is in.
• Delete the angle dimension.
• Delete the .321 dimension
• Add the new height and width dimensions (both driving dimensions)
• Then when you go to add the angle dimension and the .321 dim if you still wanted it as a reference, SolidWorks will tell you, "This dimension will over-define the sketch, do you want make it a driven dimension?"
• The user will choose yes.
• Return back to the drawing.

 

Notice there are 2 dangling dimensions to clean up as shown in Fig 14-2

Fig 14-2

After deleting the two (2) dangling dimensions, doing another insert model items will finish up the rest of the drawing.  As
show below in Fig 14-3

Fig 14-3

That's wasn't too hard, but what if one or more of those dimensions had an equation linked to it or a note attached to it, then what.  Let's do it another way using driven and driving dimensions without deleting dims that don't need to be deleted.

Do the following: (previous instructions not needed are struck out)

• Open the part model that created the drawing.
• Edit the sketch the angle dimension is in.
• Delete the angle dimension.
• Delete the .321 dimension
• Select the .321 dimension in this example
• Right click and choose driven
• Repeat for the 45.00 deg dimensions
• Control-select both dimensions and choose parentheses from the Property Manager (if that is how your company shows reference dimensions)
• Now add the new height and width dimensions (both driving dimensions)
• Then when you go to add the angle dimension and the .321 dim if you still wanted it as a reference, SolidWorks will tell you, "This dimension will over-define the sketch, do you want make it a driven dimension?"
• The user will choose yes.
• Return back to the drawing.                                                              
• Insert Model items again.

 

Notice there weren't any dangling dimensions this time to have to delete, only "Insert Model Items" again because we have added new dimensions to the model that we need to reflect on the drawing. 

 

The only problem with this way of doing drawings, that I can find is, SolidWorks for some reason will not transfer the parentheses from a changed to driven dimension, to the drawing.  So you need to remember to add the parentheses to the newly made driven dimensions.

 

The positive note in this change is, when a request for change comes for one or both of the new .771 dimensions, (and you know it will).  Straight from the marked up drawing you can change the dimensions, save and go on to the next project or drawing.

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