One of the advantages of SolidWorks is its ability to define and capture design intent within part and assembly documents.
The purpose of this approach is three-fold:
- Dimensions are reused to create the drawing. Otherwise, the sketches are dimensioned to create the part features and then recreated to create the drawing document. This is wasted effort that typically adds no value.
- Design intent is captured at the time the part is being designed, not later as an afterthought when creating a drawing. Why not spend a little time when creating the part features and drive the downstream use (drawings) from the source?
- Tolerances and annotations are defined and stored within the part features. This is better than recreating the dimension on the drawing and then adding a tolerance to the drawing dimension. The other advantage is the tolerances are shown and maintained within the sketch (figure 1).
Figure 1 - Example part with sketch dimensions and model annotations
Additional annotations -- for example, datums, datum targets, surface finish, weld symbols, and notes -- can also be defined at the part level and reused on the drawing. Figure 1 has datums and surface-finish annotations that are later reused to create the drawing views, as you'll see below.
It all starts with the part
The place where design intent is first captured is in the sketches that are used to create part features. The first step is to create a good sketch, and the way the sketch is created is important. The order of steps to create the sketch and its features are as follows:
- Create the geometric relations. Figure 1 shows the defined geometric relations. This helps reduce the number of dimensions needed to fully constrain the sketch. Creating the geometric relations first allows for the sketch to function (that is, resize) as intended (design intent). One way to see if the sketch modifies as intended is to add the geometric relations and then drag the sketch geometry to determine if the sketch is geometrically constrained properly. Geometric constraints are added by sketching (automatic) and by using the Add Relation function.
- Create the dimensions. This may include driving and driven dimensions. The driving dimensions are shown in black (figure 2). The driving dimensions will modify the sketch geometry as they are changed. The extra dimensions that are added to a sketch for reference or so they can be included in the drawing are the driven dimension shown in gray. A driven dimension cannot be modified as it is driven from the existing sketch (geometric) relations and driving dimensions.
Figure 2 - A sketch with geometric relations and dimensions
- Add the tolerances and notes within the dimensions. This attaches the tolerance directly to the sketch dimension.
- Clean up the sketch. That way, the sketch reflects what will be shown on the drawing. Figure 2 shows the dimensions spaced as they will be shown in the drawing. When the model dimensions are added to the drawing they will appear just like they looked within the sketch.
To complete the sketch, the two overall dimensions were added as driven dimension and tolerances were placed on those dimensions. Text was also added to the R.350 dimension showing it was in three places. When modifying a driving dimension, there is a default option, "Mark dimension to be imported into a drawing" or right click, and select Mark For Drawing, which can be unselected so it does not appear automatically when using the Model Items function. In this example, all dimensions were marked for use within the drawing. If a dimension is not marked for import, the text color of the dimension will change.
Reusing the dimensions and annotations
After you've added dimensions and annotations to the part to capture the design intent, you can import them into the drawing using the Model Items function. This function can be started by selecting the Model Items toolbar button (figure 3) -- this button can be added to the toolbar using the Customize function -- or select Model Items from the Insert pull-down menu.
Figure 3 - Model Items toolbar button
Once you launch the Model Items function, you'll see the Model Items options (figure 4). A couple of items to note; make sure the Selected feature is set as the source and pick the features in the view you want the dimension, and select the type of dimensions, annotations, and reference geometry you want to display. These options will be remembered for the next time you select this function.
Once the features are selected, you can move or hide the dimensions shown. Holding down the left mouse button you can move a selected dimension, and holding down the right mouse button you can hide the selected dimension. Continue this process with each feature until the drawing is complete (figure 5).
If the tolerance values, dimension precision, or dimension text is changed, the changes will be reflected within the part. Conversely, if the model changes, those changes are automatically updated on the drawing. No need to redo work on either side. If dimensions are added to the drawing, they are not included with the part.
Reusing model dimensions and annotations not only helps to reduce redundant effort but also helps to capture the design intent where it counts -- in the part features. This practice will make for better, faster designs.
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