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SolidWorks Tips & Tricks sponsored by SolidWorks for the Sheet Metal Guy

Using SolidWorks Vent Feature for Sheet Metal

The Vent command is a unique way to create sheet metal cutouts. Think of the vents for cooling fans on your computer. What would have been a long process to sketch is greatly simplified by this feature. To demonstrate an example, create a sheet metal Base-Flange. Next, create a sketch of the vent that you want to create, as shown in Figure 1.

Vent Sketch
Figure 1

With the sketch selected, click the Vent icon in the "Sheet Metal" toolbar, or pull down the “Insert” menu and pick Fastening Feature – Vent. In the Vent PropertyManager, the face is automatically selected on which to place the vent. The outside 3" circle is selected for the Boundary. Click in the box under Ribs. Then, in the graphics area, pick the four lines, as shown in Figure 2. Set the width of the ribs to ‘.125’.

Vent Ribs
Figure 2

In the Vent PropertyManager, click in the box under Spars. Then, in the graphics area, pick the 2.375" diameter circle, as shown in Figure 3. Set the width of the spars to ‘.125’.

Vent Spars
Figure 3

In the Vent PropertyManager, click in the box under Fill-In Boundary. Then, in the graphics area, pick the 1.75" diameter circle, as shown in Figure 4.

Vent Fill-In Boundary
Figure 4

In the Vent PropertyManager, under Geometry Properties, set the radius for the fillets to '.125', as shown in Figure 5.

Vent PropertyManager
Figure 5

Click the green check mark button at the top of the Vent PropertyManager to accept the settings and create the feature. Below is the final feature.

SolidWorks Vent Feature

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