SolidWorks 2011 Parts Bible - Matt Lombard [69]
Figure 4.12
Using the prompt to close a sketch setting
6. Click the Extrude tool on the Features toolbar. Answer yes to the prompt, and double-click the face of the previous extrusion. SolidWorks automatically uses the face that you double-clicked for an Up to Surface end condition. This is a simple way of linking the depths of the two extrusions automatically. Again, this entire operation could have been handled more quickly and efficiently with a cut, but these steps demonstrate an alternative method, which in some situations may be useful.
Using the Hole Wizard
The next features that you will apply are a pair of counterbored holes. SolidWorks has a special tool that you can use to create common hole types, called the Hole Wizard. The Hole Wizard helps you to create standard hole types using standard or custom sizes. You can place holes on any face of a 3D model or constrain them to a single 2D plane or face. A single feature created by the Hole Wizard may create a single or multiple holes, and a feature that is not constrained to a single plane can create individual holes originating from multiple faces, non-parallel, and even non-planar faces (holes may go in different directions). All holes in a single feature that you create by using the Hole Wizard must be the same type and size. If you want multiple sizes or types, you must create multiple Hole Wizard features.
To apply counterbored holes to your part, follow these steps:
1. Select the face that the groove feature was created on, and click the Hole Wizard tool on the Features toolbar. Then set the hole to Counterbored, set the type to Socket Head Cap Screw, the size to one-quarter, and the end condition to Through All, as shown in Figure 4.13.
Figure 4.13
The Hole Wizard Hole Specification interface
2. Next, click to select the Positions tab at the top of the PropertyManager. This is where you place the centerpoints of the holes using sketch points. It is often useful to create construction geometry to help line up and place the sketch points. Make sure the plane or face that the holes originate from is selected in the Positions tab.
3. Draw two construction lines, horizontally across the part, with Coincident relations to each side. Select both lines and give them an Equal relation. The point of this step is to evenly space holes across the part without dimensions or equations.
Tip
Although several methods exist to make multiple selections, a box or window selection technique may be useful in this situation. If the box is dragged from left to right, only the items completely within the box are selected. If the box is dragged from right to left, any item that is at least partially in the box is selected.
Tip
SolidWorks displays an error if you try to place a sketch point where there is an existing sketch entity endpoint. If you build construction geometry in a sketch and want to place a sketch point at the end of a sketch entity, you have to create the sketch point to the side where it does not pick up other incompatible automatic sketch relations, and then drag it onto the endpoint.
4. Place sketch points at the midpoint of each of the construction lines. If there is another sketch point other than the two that you want to make into actual holes, delete the extra points. Dimension one of the lines down from the top of the part, as shown in Figure 4.14. All the sketch relation icons display for reference. Click OK to accept the feature once you are happy with all the settings, locations, relations, and dimensions.
Figure 4.14
Placing the centerpoints of holes
Cutting a slot
The Hole Wizard does not specifically enable you to cut slots. However, SolidWorks