SolidWorks 2011 Parts Bible - Matt Lombard [231]
To move a dimension to another view, you can Shift+drag it from one view to the other (make sure that the dimension is appropriate in the destination view). To copy a dimension, you can Ctrl+drag it. If you cannot place the dimension in the view that you have dragged it to, then the cursor will indicate this with a special cursor symbol.
FIGURE 17.2
The default placement of dimensions into all views
If you approach this task by placing dimensions on a per-feature or per-view basis, it does not change the number of dimensions that you will have to move; it just means that you will insert fewer dimensions several times. Keep in mind that if you choose this method, there is a significant amount of cleanup and checking that you must do. The convenience of having the dimensions put into the views for you and the ability to actually change the model from the drawing are quite useful, but you may not save very much time or effort by doing things this way.
Using reference dimensions
One alternative to automatically inserting all model dimensions is to manually place reference dimensions. You create reference dimensions by using the regular Smart Dimension tool. At first, this appears to be simply re-creating work that you have already done, and this is somewhat true, but there is more to the story.
These dimensions are not duplicates of the model items. In fact, the reference dimensions that you manually place on the drawing are completely different from the dimensions that are used in the model. The dimensions serve completely different purposes in the two settings.
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 whatsoever. 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