Part V: Creating Drawings
When modeling, I tend to dimension symmetrically, but only on one side, which would not be
shown on a manufacturing or inspection drawing. I frequently use workarounds to avoid some
special problem that forces a different model dimensioning scheme than I would prefer to use.
Often, a feature is located from the midpoint of an edge, which involves no dimensions whatso-
ever. Sketch entities may have Equal relations, which also leave sketch elements undimensioned.
Dimensions may lead to faces or edges that are not in the final model or to faces that are later
changed by scale, draft, or fillets. Beyond that, when draft is involved, as is the case with plastic or
cast parts, the dimensions of the sketch that you used to create the feature often have little to do
with the geometry that is dimensioned on a print for inspection or mold building. Dimension
schemes in models reflect the need for the model to react to change, while dimension schemes in
drawings reflect the manufacturing or inspection methods, in order to minimize tolerance stack-
up, and to reflect the usage of the actual part.
Although there are strictly technical reasons for dimensioning drawings independently from the
way the model was dimensioned, there are other factors such as time, and the neat and orderly
placement of dimensions. Time is an issue because by the time you finish rearranging dimensions
that were inserted automatically from the model — checking and eliminating duplicates and then
manually adding dimensions that were left out or that had to be eliminated because they were
inappropriate for some reason, as well as ensuring that all the necessary dimensions are on the
drawing — it would have been much quicker to manually dimension the drawing correctly the
first time using reference dimensions.
In most cases, inserting model dimensions into the drawing is impractical for manufacturing or
inspection drawings unless you have simple plates with machined holes. This is because of the
amount of time required to rearrange and check the dimensions, the need to ensure that you have
placed the necessary dimensions and taken geometric tolerancing into account, and the simple fact
that the dimensioning and sketch relations needed for efficient modeling are usually very different
from the dimensioning needed for manufacturing or inspection.
I recommend that you use the manual dimension placement option, which works much in the same
way as when dimensions are added to sketches. Dimensions that you place in the drawing in this
way are called driven, or reference, dimensions. In drafting lingo, reference dimensions are “extra”
dimensions that you place to ease calculations, and you usually create these dimensions with paren-
theses around them; in SolidWorks lingo, reference dimensions are simply driven rather than driv-
ing dimensions. To find the setting that controls the parentheses around reference dimensions,
choose Tools ➪ Options ➪ Document Properties ➪ Dimensions ➪ Add Parentheses By Default.
Rapid Dimension
A new feature in SolidWorks 2010 is Rapid Dimension, which offers a manipulator wheel that
shows the possible locations of a dimension you are trying to place.
Rapid Dimension works for dimensions inside drawing views, not on dimensions on the sheet. It
enables you to choose from either two or four options, and you can move between the options
with the Tab key, making your selection with the Spacebar. You can also left click on the manipu-
lator to select an option The Rapid Dimension manipulator wheel is shown in Figure 23.3 in the
placement of diameter and linear dimensions.
