Alibre Options: Using Boolean Operations in a Part Workspace

Boolean operations can help you create or modify parts or assemblies.

They consist of two main components. First are the tools -- one or more parts and assemblies. These tools are used to modify the second component, the blank, which is the part that you are currently working on. This month we'll focus on using Boolean operations to create Design Boolean features.

In a part workspace, Boolean operations are performed in a special mode called the Design Boolean Editor Environment. Design Boolean features are associative, meaning that if you modify and save the original parts/assemblies that were used as tools, the Design Boolean feature(s) update when you reopen the design that contains them.

The three Design Boolean features are: Boolean Unite, Boolean Subtract and Boolean Intersect.

Part 1: Creating a Boolean Subtract Feature
1. Open or create a part that serves as a blank. In this example I created a simple cylinder block by drawing a circle with a 4.5" diameter; then I used the Extrude Boss tool to extrude it to a 5" cylinder (figure 1).

Figure 1. The cylindrical block example that I'll use for the Boolean operation.

I'll perform a Boolean subtract operation by taking a standard screw and using it to drill a threaded hole on a cylindrical block. When you do a Boolean subtract, you take a tool and use it to carve out your blank.

2. Locate the Boolean Unite tool on the Features toolbar and click the flyout button icon to see all three options including Boolean Subtract and Boolean Intersect .

3. Select the Boolean Subtract tool. The part workspace switches to the Design Boolean Editor Environment (figure 2).

Figure 2. The Design Boolean Editor Environment.

The editor looks very similar to the assembly workspace and has some of the same editing tools. Once the Editor is activated, the Insert Part/Subassembly dialog box appears (figure 3).

Figure 3. The Insert Part/Subassembly dialog box allows you to select the tool to use for the Boolean operation.

4. Select the part you want to use as a tool to define what the program will remove from the blank. For this example, I will use a simple threaded screw from the part library. If you don't have access to a part library, you can select another part or create your own screw. For more information about the features needed to create a screw, review the tutorials under Part Design called Modeling a Simple Part and Creating Helical Geometry.

5. Generally the Boolean Subtract feature should be slightly wider than the tool. To scale the screw, select Feature / Scale. Check the uniform check box and set the scale factor to something slightly bigger such as 1.2 (figure 4). Save these changes.

Figure 4. Set the scale to a factor slightly bigger than 1 to account for the size of the hole.

6. Click the work area to place the tool in any convenient location close to the blank (figure 5). To place more copies of the part, continue to click the work area.

Figure 5. You can insert as many copies as needed on the workspace by clicking the work area.

When you are done click the Finish button (figure 6).

Figure 6. Click the Finish button when you are done inserting copies of the part.

7. Position and constrain the tools as necessary. In this example I will use the Boolean Subtract feature to drill four holes by constraining four screws to the cylinder. Rather than inserting and constraining four screws individually, I'll use a pattern feature. a. To move the screw, select a planar surface and select the Move tool . A tri-directional arrow will appear (figure 7).

Figure 7. Pick any of the directional arrows to choose the direction to move the part.

b. Click one of the arrows to select the direction that you want the part to move; then drag the part over the planar face of the cylinder. When you finish, click the Move tool again to release it.

You may also use the Rotate tool to rotate the part if needed. In this case the tri-directional arrow represents the axis of rotation for the part.

8. Using the Assembly Constraint tools, I will precisely place the part on the blank. Because the screw doesn't have many planar surfaces to use for constraints, use its reference geometry instead.

a. In the Design Explorer, right-click the screw and select Show Reference Geometry (figure 8).

Figure 8. The reference geometry is the geometry that corresponds to the original part or assembly. It is independent of the workspace geometry.

b. Select the Assembly Constraint tool and constrain the screw to the cylinder.

9. To pattern the screw, click the flyout button below the Linear pattern icon and select the Circular Pattern tool or go to Insert / Part/Subassembly Pattern / Circular.

10. Click in the Part/Subassembly to Pattern field , and select the screw in the workspace. Click in the Center field and select the central axis of the cylinder for the center, in this case the z-axis on the workspace. The number of copies is four, including the original, and the angle is 90