Alibre Options: Create a Feature Catalog

6 Nov, 2006 By: Michael Todd

Reusing common features is easy with the Catalog feature.

This month we'll cover a useful feature in Alibre Design -- the Catalog tool. Alibre Design offers the ability to reuse common features in different models. The advantage of this is that you can create a catalog of common parts that is readily available, such as a specific shape that you sketch frequently to create an extruded cut in a model. By reusing a part you can rest assured that the feature is using the correct dimensions, as well as reducing your design time.

The following types of features can be cataloged and used again: extrude boss, extrude cut, hole, sheet-metal cut and sheet-metal dimple, and sketches.

Creating the Feature

  1. Create a 3D model that you want to place a pattern on. Figure 1 shows a sheet-metal plate (approximately 10" X 4") that uses common cutouts to insert latches.

Figure 1. A sheet-metal part about 10" X 4".

  1. In the work area, select the face to use as the sketch plane -- the face is highlighted in a different color when selected -- and then select the Activate 2D Sketch tool.
  2. Sketch the profile for the feature you wish to create. Figure 2 shows a profile for a sheet-metal cut.

Figure 2. A profile of a sheet-metal cut.

  1. Create a 3D feature from the sketch. (Make sure that you choose one of the features mentioned in the introduction that can be cataloged.) Figure 3 shows the sheet-metal cut created from the profile in figure 2.

Figure 3. Sheet-metal plate with cut.

Save the Catalog Feature

  1. Once you have a feature to catalog, you're ready to save the feature. From the Feature menu, select Save Catalog Feature, and the Save Catalog Feature dialog box appears.

Figure 4. The Save Catalog Feature dialog box.

  1. Check the Exported Feature field, and then select the feature (or sketch) that you want to save from the Design Explorer. In figure 4 above, the feature Cut <4> is selected.
  2. Click the Save As button and the Save As dialog box appears.

Figure 5. The Save As dialog box.

  1. Browse to find a location you wish to store the catalog feature. You can save to the Repository (if you have a license for it) or within Windows File System. In this example, the feature is stored in a folder in the repository called Catalog Features.
  2. In the Name field, enter a distinguishing name for the feature and select Save.

Using the Catalog Feature

  1. Once the feature is saved, you can use it again as often as you like. From the Feature menu, select Insert Catalog Feature.

Figure 6. The Insert Catalog Feature dialog box.

  1. In the Insert Catalog Feature dialog box, select Catalog Feature field and click the Browse button Browse button to locate the catalog feature you saved.
  2. In the Placement section, you can specify how you want the feature to be laid out on your model. In the Base Plane field, select the face (or plane) that you want to place the feature on. In Alignment Reference, you can select a linear edge to orient the feature.

Note that how the feature is placed depends on how you originally created it. The original alignment reference is the bottom of the window when the sketch was created. Therefore, the bottom of the feature as the profile was sketched is aligned with the edge chosen here.

In this example, the Alignment Reference remains blank because the preview is in the correct orientation for this design.

Figure 7. The sheet-metal part with the preview of the inserted feature.

  1. If you need to rotate the feature, you can enter a value for degrees of rotation in the Rotation field, or you can use the Rotate and Move handles on the preview. Move your mouse pointer over the handles until the Move or Rotate arrows appear, then click and hold to drag the preview around.

Figure 8. The preview of the inserted feature showing the Move handle.

Figure 9. The preview of the inserted feature showing the Rotate handle.

  1. When you are satisfied with the general placement, select Apply to place the feature. The dialog remains open, so you can place another feature as needed. You can place the same feature again or choose a different one. When you have finished placing additional features, choose Close.
  2. Notice the Catalog Feature is now listed in Design Explorer.

Figure 10. The Design Explorer showing the new catalog feature.

  1. You can now edit the sketch that was created with the Catalog Feature to more precisely locate the feature on your model. Note that it may be necessary to delete some of the references that were created automatically in the sketch in order to place new driving dimensions.

Using the Catalog Feature, we have successfully reused a common feature that may appear in multiple designs, saving time because the sketch and the feature only have to be created one time.

Be sure to read next month's Alibre Options column, where we will explore another great feature of Alibre Design. Until then, look for me as the Alibre Assistant online in Alibre Design.

About the Author: Michael Todd

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