SolidWorks 2011 Parts Bible - Matt Lombard [19]
• Locked
• Broken
• Selected Entities
In the lower Entities panel of the Display/Delete Relations PropertyManager, shown in Figure 1.26, you can also replace one entity with another, or repair dangling relations.
FIGURE 1.26
The Display/Delete Relations PropertyManager enables you to repair broken relations.
Cross-Reference
You can read more about repairing dangling entities in Chapter 12.
Using suppressed sketch relations
Suppressing a sketch relation means that the relation is turned off and not used to compute the position of sketch entities. Suppressed relations are generally used in conjunction with configurations.
Cross-Reference
Configurations are discussed in detail in Chapter 11.
Working with Associativity
In SolidWorks, associativity refers to links between documents, such as a part that has an associative link to a drawing. If the part changes, the drawing updates as well. Bidirectional associativity means that the part can be changed from the part or the drawing document window. One of the implications of this is that you do not edit a SolidWorks drawing by simply moving lines on the drawing; you must change the model, which causes all drawing views of the part or assembly to update correctly.
Other associative links include using inserted parts (also called base or derived parts), where one part is inserted as the first feature in another part. This might be the case when you build a casting. If the part is designed in its “as cast” state, it is then inserted into another part where machining operations are performed by cut features and the part is transformed into its “as machined” state. This technique is also used for plastic parts where a single shape spans multiple plastic pieces. A “master part” is created and split into multiple parts. An example would be a mouse cover and buttons.
One of the most important aspects of associativity is file management. Associated files stay connected by filenames. If a document name is changed, and one of the associated files is not updated appropriately, the association between the files can become broken. For this reason, you should use SolidWorks Explorer to change names of associated files. Other techniques will work, but there are some techniques you should avoid.
Best Practice
It is considered poor practice to change filenames, locations, or the name of a folder in the path of documents that are referenced by other documents with Windows Explorer. Links between parts, assemblies, and drawings can be broken in this way. Using SolidWorks Explorer or a PDM application is the preferred method for changing filenames.
On the DVD
Refer to the DVD to find video tutorials for Finding Help, Parametric Sketching, and Working with Templates.
Tutorial: Creating a Part Template
This simple tutorial steps you through making a few standard part templates for use with inch and millimeter parts, as well as making some templates for a couple of materials.
1. Choose Tools⇒Options⇒System Options⇒File Locations and then select Document Templates from the Show folder for list.
2. Click the Add button to add a new path to a location outside of the SolidWorks installation directory where you have copied the templates from the DVD with this book; for example, D:\Library\Templates.
3. Click OK to dismiss the dialog box and accept the settings.
4. Choose File⇒New from the menu.
5. Select any part template.
6. Choose Tools⇒Options⇒Document Properties⇒Drafting Standard.
7. Make sure the ANSI standard is selected.
8. Click the Units page.
9. Change the unit system to IPS, inches with three decimal places, using millimeters as the dual units with two decimal places. Set angular units to Degrees with one decimal place.
10. Change to the Grid/Snap page.
11. Turn off Display grid.
12. Change to the Image Quality page.
13. Move two-thirds of the way to the right, so it is closer to High. Make sure the Save tessellation with part document option is selected.
14. Click OK to save the settings and exit the Tools⇒ Options