Page 172 - Mastering SolidWorks

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Creating a Simple drawing 141

Reference (driven) Dimensions can be applied to the drawing view directly. These are
only associative in one direction, meaning that they measure what is there, but they do
not drive the size or position of the geometry. All changes must be made from the model.
Again, on the face of things, this appears to be redundant and a waste of time; but in my
personal estimation, by the time you finish rearranging dimensions, checking to ensure
that you have everything you need, and hiding the extraneous dimensions, you are usu-
ally far better off using reference dimensions.

Best Practice
Users have strong opinions on both sides of the issue of dimensioning drawings. the best thing for
you to do is to use both methods and decide for yourself.

17. If you choose to use the Model Items approach, you can do this by choosing Insert ➢
Model Items. Specify whether the dimensions should come from the entire model or just a
selected feature. You also need to ask whether the dimensions should come into all views
or just the selected one, and whether you want just a certain type of dimension, annota-
tion, or reference geometry.
18. After the dimensions are brought in, you need to move some of them from one view to
another, which you can do by Shift+dragging the dimension from the old location to the
new location. Ctrl+dragging predictably copies the dimension. You can move views by
dragging an edge in the view.

Sheet vs. Sheet Format

with new and even experienced users, there is some confusion around the Sheet versus Sheet
Format issue. part of the confusion is due to Solidworks terminology. Solidworks names the two
items Sheet and Sheet Format. in this book, i simply use the terms Sheet and Format to avoid linking
the two items with a common first name. it would be better yet if Format were changed to Border or
Title Block so that the name more closely matched the function. Just be aware that title Block has a
precise meaning in Solidworks; there are commands associated with it.
in a Solidworks drawing, you are editing a view, the sheet, or the format. when editing the sheet,
you can perform actions such as view, move, and create views, but you cannot select, move, or edit
the lines and text of the drawing border. when editing the format, you can edit the lines and text
that make up the drawing border, but the drawing views disappear. also, you can edit annotations
in the format from the sheet layer.
Often, users save a template that already contains a format to save themselves some time every time
they create a new drawing. Chapter 24 covers setting up automation of drawing creation.