Alibre Options: Using the Hole Tool in Alibre Design

Automatically place and set dimensions for the holes in your designs.

Alibre Design’s Hole feature allows you to create standard holes (i.e., counter bore, countersunk, etc.) and place them on a regular or sheet-metal part. You create the holes by entering the desired parameters in the Hole Feature dialog box and place them by left-clicking on the desired location on a face. This month, I’m going to discuss how to use the Hole tool as an effective tool in your design process.

Part -1. Create a Hole on a Part
To begin, first create a solid block (figure 1).

1. Sketch a rectangle and dimension it 4″ X 9″, then extrude it to 2.5″.

Figure 1. Create a block.

2. Select a face on the block and left-click relatively close to where you want to place the hole, then select the Hole tool on the Part Modeling toolbar. You’ll see a preview of the hole at the location you clicked on, and the Insert Hole dialog box appears.

Figure 2. The Insert Hole dialog box with the hole preview.

Note: You do not have to dimension the hole in this step. Once the hole is placed, it shows up in the Design Explorer as a sketch. You can edit that sketch at any time to position or reposition the hole.

3. Select the type of hole that you want to create. For this example I’ll select a countersunk hole. Notice how the preview of the hole changes as well as the parameter information that you can enter.

Figure 3. Select countersunk as the type of hole.

4. Enter the parameters for the hole. If you want the hole to go through the entire block, change the depth condition from Blind to Through All. This option is useful if the width of the block may change, because the hole adjusts accordingly. Sometimes you need a hole to extend to a specific surface. When this is the case, select the To Limit Geometry depth condition, then on your part, select the limiting geometry and apply an offset if necessary.

5. Finally, you can add threads to a hole. Many predefined threads are already in the Series drop-down list. Note that when you create a thread, it’s not graphically represented on the model. However, when you create a 2D drawing, the thread information is displayed on the applicable orthographic view.

Figure 4. Threads in a 2D drawing.

In addition to predefined thread options, you can create your own thread definitions by editing the Alibre Design thread definition file, ALIBRE_UNICODE.THD in Notepad. It contains a definition of the file format that you need to create the custom thread. The file is located at C:\Documents and Settings\All Users\Application Data\Alibre Design\System Files.

6. Now that you have selected all the desired parameters, you can select OK on the Insert Hole dialog box, or you can left-click on the model to place additional holes. Every time you click on a face, Alibre Design generates a preview of a hole. Place three additional holes on the remaining three corners of the surface. To move the holes around, use the Select tool on the Sketch toolbar on the right, then select a center node and drag it around. You can also delete an unwanted hole by selecting it and pressing Delete on your keyboard.

Figure 5. A block with four holes.

7. Next, you can constrain the holes appropriately before you select OK or you can edit the sketch that is created under the Hole feature on the Design Explorer to edit and constrain the hole(s) afterwards. If you edit the hole sketch later, you won’t be able to see the hole previews — only their center nodes display in the sketch. In this example, I’ll dimension the center nodes to the edges of the block so that all the holes are aligned properly. Dimension all holes so that they have the same distance from their centers to the edge of the model.

Figure 6. Holes are all aligned and show dimensions.

8. Finally, click OK on the Hole dialog box and the result should look something like this:

Figure 7. Final block with holes.

Part 2. Create a Hole on a Cylindrical Part
Creating a hole on a part usually entails starting with a flat face, however sometimes it’s necessary to create a hole on a cylindrical face. To achieve this, follow these instructions.

1. First, create a hollow cylindrical tube by sketching two concentric circles centered about the origin. Dimension one 4.5″ and the other 5″. Next extrude the sketch 7″. The tube should look like the illustration below.

Figure 8. Cylindrical tube.

2. Create a plane tangent to the surface. Go to Insert / Plane. Select a plane of reference, such as the yz-plane, and the outside surface of the tube and then press OK.

Figure 9. Plane tangent to tube.

3. Now highlight this new plane and select the Hole tool. You won’t see a preview because a surface was not selected; however, you can select a position on the plane to create a preview. In this example, I’m selecting two points tangent to the plane. As soon as you select the points on the plane, you’ll see a preview of the holes. Verify that they are not facing outward. If they are, click on the Reverse checkbox on the Hole dialog box. For the limiting geometry, select the inner surface of the cylinder with an offset of 0.2″ so that the hole goes through the wall of the cylinder. Then dimension the holes so that they are each 1″ from the edge of the ends.

Figure 10. Cylinder with holes.

4. Click OK to accept the changes. The cylinder with holes should look like the figure below.

Figure 11. Final cylinder with holes.

If you need to, you can use the Pattern feature to create multiple holes around the cylinder. Go to Feature / Pattern / Circular. Select the Hole as the feature to pattern and the central axis of the cylinder for the Center, then choose the number of copies (including the original) and the degrees of rotation between copies. Here’s an example of what it could look like.

Figure 12. Cylinder with patterned holes

This concludes this demonstration of the Hole tool. Use this knowledge to make cleaner drawings and improve your designs.

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