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• The commands that can merge bodies in sheet metal parts are as follows:

• Edge Flange

• Combine

The Mirror function enables you to mirror bodies, but the new bodies have to be merged manually with the existing body.

Using Insert Part

Using the Insert Part feature inserts an existing part as a new body inside a sheet metal part, but even if the inserted part was a sheet metal part initially, it does not show up as sheet metal after being inserted in the other part.

You can join the inserted part to the local sheet metal body by using the Combine feature, but not by using the merge option in an Edge Flange as you can to merge two bodies modeled within a single part. When the Combine feature is used, any sharp intersection between the parts is left sharp and will not flatten unless you use the Insert Bends feature to convert the sharp into a bend. This is an odd twist on combining the old (Insert Bends) method with the new (Base Flange) method.

Using multiple Base Flanges

Another method to get multiple bodies inside a sheet metal part is to start from disjoint Base Flange features. You can build flanges toward one another until flanges touch. Figure 21.45 illustrates a situation where a disjoint flange created by a Base Flange feature is connected to the main part using an Edge Flange feature with the Up To Edge And Merge flange length setting.

FIGURE 21.45

Using an Edge Flange to connect disjoint bodies in a sheet metal part

Tutorial: Working with the Insert Bends Method for Sheet Metal Parts

The Insert Bends method has been relegated to duty mainly for specialty functions. To gain an understanding of how this method works, follow these steps:

1. Create a new blank part.

2. On the Top plane, open a sketch and sketch a rectangle centered on the Origin 12 inches in the Horizontal direction and 8 inches in the Vertical direction.

3. Extrude the rectangle 1 inch with 45 degrees of draft, Draft Outward, in Direction 1, and extrude 1 inch with no draft in Direction 2. The two directions should be opposite from one another.

4. Shell out the part to .050 inches, selecting the large face on the side where the draft has been applied. The part should now look like Figure 21.46.

5. Use the Rip feature to rip out the four corners. Allow the Rip to rip all corners in both directions. The part should now look like Figure 21.47.

Figure 21.46

The part as of Step 4

Figure 21.47

Ripping the corners

6. Create an Insert Bends feature, accepting the default values, and picking the middle of the base of the part for the fixed face.

7. Draw a rectangle on one of the vertical faces of the part, as shown in Figure 21.48.

8. Use the sketch to create a Through All cut in one direction. Notice that the Normal cut option is on by default. Examine the finished cut closely; notice that it is different from the default type of cut because it is not made in a direction normal to the sketch but rather in a direction normal to the face of the part. Details of this are shown in Figure 21.49.

Figure 21.48

Ripping the corners

Figure 21.49

Using the Normal cut option

9. Click the Flatten button on the Sheet Metal toolbar. Notice that the Flat Pattern feature becomes unsuppressed and that the Bend Lines sketch under it is shown. This works just like it did in the Base Flange method. The finished part is shown in Figure 21.50.

Figure 21.50

The finished part with the Flat Pattern feature unsuppressed

Tutorial: Using the Base Flange Sheet Metal Method

SolidWorks Base Flange method for sheet metal is fun and easy to use, as you will see in this tutorial:

1. Open a new part using a special sheet metal template if one is available.

2. On the Top plane, draw a rectangle centered on the Origin, 14 inches in X by 12 inches in Y (or Z).

3. Initiate the Base Flange tool, set the thickness to .029 inches, and change the K-Factor to .43. Notice that the default inside bend radius is not shown. This setting is made in the Sheet Metal feature that is placed