Part IV: Creating and Using Libraries
Understanding Dissection
Dissection is a process that SolidWorks goes through by which it examines all the parts on your
computer and makes Design Clipart of the sketches and features. People who might get some use
from this function are those who have not modeled a lot of parts and will tend to reuse the same
features over and over again. The types of data it will try to recycle for you are extrudes and cuts,
sketches, blocks, and tables from drawings.The first interaction most people have with this function is learning how to turn it off. If you notice
your computer starting to run small SolidWorks windows in the background starting at about
11 pm daily, you may have Dissection turned on. To select or deselect Dissection, choose Tools ➪
Options ➪ Search. Dissection is connected to SolidWorks Search, another function many users
prefer to deselect.Tutorial: Working with Library Features
This tutorial guides you through customizing a Hole Wizard hole to use as a specialty library fea-
ture, then storing it in the library, editing it, and placing it in a part. Follow these steps:- Open a new part, and create a rectangular base feature, about three inches high by
three inches wide and three inches deep. - Pre-select a flat face and start the Hole Wizard.
- Create a counterbored hole for a Heavy Hex Bolt,^1 ⁄ 2 -inch, Normal Fit, Blind,
1.2 inches deep. Locate the hole with dimensions from two perpendicular edges, as
shown in Figure 18.15. Click the green check mark icon twice to accept the hole settings. - Turn on the setting at View ➪ Dimension Names.
- Double-click the counterbored hole feature in the FeatureManager to show the
dimensions. Make sure Instant3D is unselected for the next step. - Click one of the dimensions that you created to locate the center of the hole and
rename the dimension in the Dimension PropertyManager (Primary Value panel)
using names that will have meaning when you place the dimension, such as XDir,
or YDir. Do this for both dimensions. - Edit the second sketch of the hole. Figure 18.16 shows what the sketch should look
like before and after the edit.
Caution
Do not delete any of the named dimensions in a normal or revised Hole Wizard hole. SolidWorks has a check-
ing mechanism that looks for these names and will display an error if any of the named dimensions is not there.
If there is no use for the dimension, it still has to be there, although it does not need to be used for its original
use. You could rename another dimension with the name or simply dimension the length of the centerline or
an otherwise unused construction line. It does not matter about the function of the dimension, as long as there
is a dimension with that name in the sketch. n