SolidWorks 2011 Parts Bible - Matt Lombard [203]
FIGURE 14.9
Custom property formatting in the title block
The syntax $PRP or $PRPSHEET indicates that the property that follows the syntax is to be pulled from either the current document (drawing) or from the model specified in the Sheet Properties, respectively. This is an important distinction to make. Most of the time, you can type custom properties in at the part or assembly level so that you can reuse the data by drawing properties, BOM, or even design tables.
Notice that all the notes in the format that are showing raw syntax are pulling data from the model. “Draw2” and the Scale notes are driven by the drawing. When no value exists for the property to display, you have an option of what to show. The top portion of Figure 14.10 shows the settings in the View menu that control the display of syntax of the custom property links. In general, it is common to deselect the error display and to show the link variables.
FIGURE 14.10
The link variable's display options and effects
Displaying errors and link variables
The errors in Figure 14.10 are caused by links to the local document for which there is no corresponding property. For example, the “ERROR!: COMPANYNAME” message is linked to “$PRP: COMPANYNAME,” but the local custom property COMPANYNAME does not exist. If it existed but had a null or space value, the error would disappear.
Likewise, with the option to display link variables selected, the syntax that calls model custom properties displays until there is some value for it to pull from. If a part is put onto the drawing, then some of the properties are filled in because properties and values exist to pull from, and the rest of the properties simply disappear to make space. Notice in Figure 14.11 that the Material property has been filled in, but the Finish property has not. This is because either there is no Finish property in the part on the drawing or there is a null value in the Finish property.
FIGURE 14.11
Custom properties filled in by a part
Tip
When initially setting up the format, it can be useful to have a dummy model already on the drawing. The dummy model should have all the custom properties in it that you intend to use in your drawings. This prevents the blank fields or error messages from appearing during setup.
Note
If you drag-and-drop a part onto a drawing while editing in the Sheet Format, the views may appear for a split second and then disappear again. This is because you cannot display drawing views while editing the Sheet Format. Once you exit the Sheet Format and go back to editing the sheet, the views can display once more.
Creating linked properties
It is easy to create annotations that are linked to properties. Begin as if you are creating a note:
1. Click the Note toolbar button on the Annotations toolbar, or choose Insert⇒Annotations⇒Note.
2. Place the note on the drawing. The Formatting toolbar appears.
3. Click the Link to Property button in the Text Format pane of the Note PropertyManager. This displays the Link to Property dialog box, as shown in Figure 14.12, which gives you the option of linking to a custom property in the current (drawing) document or in the model (part or assembly) that is on the drawing.
Figure 14.12
The Link to Property dialog box
4. If the desired custom property is not in the drop-down list shown to the right, then you can type it into the text box or click the File Properties button to edit the properties. If the property is added to the part file or a part file with that property is used on the drawing, this linked annotation will pick it up. This button is not available for the model if there is no model on the drawing, in which case you must type in the name of the property manually.
Using the Title Block function
The Title Block enables the person who sets up the sheet format to specify an area that contains notes that are easy to access without editing the format. (Many CAD administrators prefer that the users not have to deal with the details inside the Sheet Format.) You can even