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 18.14. Click the green check mark icon to accept the hole settings.

Figure 18.14. Placing a hole

Select ToolsOptionsGeneral, and turn on Show Dimension Names.

Double-click the counterbored hole feature in the FeatureManager to show the dimensions. RMB click one of the dimensions that you created to locate the center of the hole, and select Properties.

Rename the dimension using different names, so that they 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 18.15 shows what the sketch should look like before and after the edit.

Do not delete any of the named dimensions in a normal or revised Hole Wizard hole. SolidWorks has a checking mechanism that looks for these names, and it will display an error if the named dimension 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 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.

You should also name any new dimensions that you may want to change. These dimensions will have more meaning when you are placing the feature if they have names.

Figure 18.15. Reconfiguring the hole

Remember that to get the diameter dimensions shown in Figure 18.15 (instead of radius dimensions), you must use the dimension tool to select the centerline (construction line) and the line or endpoint on one side, and then move the cursor to the other side of the centerline to place the dimension (the order of selection does not matter). When the cursor crosses the centerline, the dimension will display as a diameter instead of a radius.

When you are done editing the sketch and renaming dimensions, exit the sketch.

Click the CBORE feature twice, or click it once and press F2, to rename it as SpecialHole.

Pre-select the same flat face that the first hole feature was placed on, and start the Hole Wizard again.

Place a #8-32 tapped hole, accept the default depth, and specify a center-to-center distance of .75 inches between it and the SpecialHole. Rename the radial dimension as MountRad.

Using the temporary axis through the center of the SpecialHole, make a circular pattern of the new tapped hole, creating a total of four instances of the tapped hole. Make the SpecialHole Feature red, and the tapped hole and pattern yellow.

Split the FeatureManager window into two by using the splitter bar at the top. Change the lower panel to the ConfigurationManager.

Rename the Default configuration to Size1.

Create a new configuration called Size2. Double-click the SpecialHole feature and change the dimension named C'Bore Dia to 1.5 inches. Be sure to change to This Configuration Only, using the drop-down menu.

Make a dimension change for the MountRad dimension to 1 inch. The results to this point are shown in Figure 18.16.

Figure 18.16. The results after step 16

Auto-create a design table by selecting InsertDesign Table, and then selecting the Auto-Create option. Edit the design table to look like Figure 18.17.

Remember that to fill the first two columns up to Size5, you can make the two-by-two selection of the Size1 and Size2 entries in the first two columns, and pull down the handle in the lower-right corner of the selection box until the appropriate boxes are filled.

Figure 18.17. The design table for the SpecialHole feature

Manually fill in the C'Bore Dia values, but in cell D3, type the equation =C3/2+.25. Then use the same Fill technique to populate cells D3 to D7.

Test the configurations to make sure that they all work.

In the Design Library, browse to a folder where you would like to put this library feature. (Make sure that it is not used by assemblies or sheet metal forming tools.) Click a face created by the SpecialHole feature, and drag the feature into the lower pane of the Design Library. The Add to Library PropertyManager should appear on the left.

Although you selected a feature and dragged it into the library, the Items to Add field appears blank. Select the SpecialHole, tapped hole, and circular pattern features, either through the split FeatureManager or the flyout FeatureManager. Selecting the features from the graphics window does not work.

Position and zoom the view of the part so that when it is saved, you see a good preview of the library feature. Also, if you have not changed your background color from blue to white, this would be a good time to do so.

In the Save To pane, make sure that you select the correct folder, then fill in a filename, and click OK. Figure 18.18 shows the completed PropertyManager interface for this function.

You may notice that there are two library entries in the window. This is because an additional path has been added in Tools Options File Locations, Design Library.

If the new library feature does not appear in the Design Library, then click in the Design Library and press F5. If you do not like the way that it displays, then RMB click in a blank space inside the lower library window and select one of the other three options.

To edit the preview image of the feature, RMB click the feature in the Design Library window, select Open, reposition or zoom the view, and save it. Click in the Design Library and press F5 again.

Figure 18.18. Saving the library feature

It is recommended that when placing a library feature, you should close the original library feature window. The workflow proceeds much more smoothly if the part is closed before you use it.

Open the part from the CD-ROM called Chapter 18 Tutorial Blank.sldprt. If you would like to examine the version of the SpecialHole part that I created, it is stored with this data as well.

Drag the SpecialHole library feature from the Design Library onto the face of the blank part. Place the feature near the squared-off end. Select a configuration from the list in the PropertyManager.

Although there is no prompt, when the Library Feature interface hesitates and there are configurations in the library feature, it is waiting for you to select a configuration. A prompt actually does exist, but it appears in the lower-left corner of the screen on the status bar in a tiny font, and most users probably do not notice it.

Try to orient the part in the same way that it appears in the preview window, as shown in Figure 18.19.

Figure 18.19. Orienting the part and selecting references

Select edges on the Blank part that correspond to the preview window. Click OK to accept the placement of the feature.

Double-click the SpecialHole feature and change the X and Y placement dimensions to place it one inch from the edges in both directions.

Place another library feature onto the blank part. Select a configuration, and click the green check mark icon, without selecting edges for the references.

Notice that the feature in the FeatureManager appears with an exclamation mark. If you investigate the cause of this, then you can see that the two dimensions that should be attached to edges are dangling because you did not select the references while placing the library feature. This was done on purpose to show a different technique.

Expand the library feature and the SpecialHole feature, and edit the first sketch in the Special Hole. This is the placement sketch. Delete the two dimensions that appear in dangling colors.

Add a concentric sketch relation between the placement point and the arc edge of the Blank part. Exit the sketch. The error message should now be gone and the hole should now be placed in the center of the arc.

RMB click the second library feature and select Dissolve Library Feature.

Figure 18.20 shows the finished part and FeatureManager. Good job!

Figure 18.20. The finished part