Solid Thinking: More Functional Features to Build Plastic Parts

SolidWorks' vent and fill pattern tools help automate the task of creating features that are functional in nature.

Unlike the fastening features, these features are built at the part level and not within the content of the assembly.

Vent
The Vent feature creates a vent in one step using a pre-defined 2D sketch (figure 1).

Figure 1. Example of the 2D sketch used to create the vent feature and the completed vent.

The different areas of a vent are shown in the left side of figure 1. These areas are defined within the Vent Property Manager and are as follows:

1. Vent boundary
2. Ribs
3. Spars
4. Fill-in area

Also note that when creating a vent feature, you need to create and display the 2D sketch used to define the vent. If you can't see or select the vent sketch, check to see if Sketches is selected under the View menu.

The first portion of the Vent Property Manager defines the boundary of the vent from a pre-defined 2D sketch, the face to place the sketch upon, draft added to the ribs, spars and fill-in area (figure 2). You can specify a radius for the sharp corners of the vent. The flow area is updated based the selections made and values defined for the vent, which gives you feedback on open area of the vent. If more area is required, you can change the overall boundary or vent features to add more open space to the vent.

Figure 2. Top portion of the Vent Property Manager.

The second portion of the Vent Property Manager defines the geometry used, width, depth, offset and direction of the ribs, spars and fill-in boundary (figure 3). The changes to the vent are shown on-screen as soon as the change is made.

Figure 3. Bottom portion of the Vent Property Manager.

Fill Pattern
Another way to get a vent-like feature in your part is to use the Fill Pattern tool. Figure 4 shows a pattern of holes created to fill into the sketch area, which lets you create a sketch to define the area of the sketch. The image on the right side of figure 4 shows the pattern that was created based on the selected pattern layout, spacing, offset from the sketch boundary and seed feature.

Figure 4. Creating a fill pattern using a 2D sketch to drive the size and location of the holes.

When using the Fill Pattern tool, the sketch used to define the boundary for the pattern is selected first (figure 5). Then describe on the pattern layout. You can select the style (perforation, circular, square or polygon) of the pattern or change it later, as well as the spacing between the holes, angle of the hole pattern, spacing from the edge of the boundary and an option.

Figure 5. Fill Pattern Property Manager for the feature.

The next main area to define is within the Feature to Pattern field. This area of the Property Manager defines the type of feature used for the pattern. You can use features already created within the part or selected from pre-defined list of features (hole, square, diamond and polygon).

If you use a selected feature, the program uses it for the pattern. The feature does not need to be, nor should it be, within the fill boundary.

Within the options area, you can select Geometry Pattern to improve performance. This option patterns only the information required to display the pattern feature without the information for each individual feature in the pattern or end conditions (up to surface, depth, etc.).

Propagate visual properties also copies color, textures and cosmetic thread information for the pattern instances.

Automatically Create Features
Use the Vent and Fill Pattern tools to help automate the task of creating features that are functional in nature.