Manufacturing

Alibre Options: Creating Exploded Views for Use in 2D Drawings

15 Jul, 2005 By: Michael Todd Cadalyst

Make the smallest parts of your designs easy to see with exploded views


Whenever you create an assembly in Alibre Design, you have the ability to create multiple exploded views, which you can insert into a figure2D drawing. An exploded view of an assembly displays the individual parts while maintaining their relative location in the assembly.

An exploded view is particularly helpful when displaying the parts of a tight assembly that might otherwise be difficult to distinguish. When placed in a 2D drawing with a BOM, an exploded view also lets you easily add callouts to the parts in the assembly.

To create exploded views for a 2D drawing:

1. Open an existing assembly. From the Alibre Design home window go to File / Open and select an assembly. For the purpose of this tech tip, it's best to start with a simple assembly.

Note: You may want to adjust the color scheme or workspace background color to a darker tone. The Exploded View Trails may be difficult to see on a light background. To adjust these settings in the Assembly workspace, select Tools / Options / click the Color Scheme tab and choose a dark background.

2. In the assembly workspace, select Insert / Exploded View.

The workspace is now in Exploded View mode. Initially the assembly will not appear exploded. All exploded views are listed under Exploded Views in the Design Explorer.

Note: The Assembly toolbar is the set of icons located by default on the right side of your assembly workspace; the Design Explorer is located on the left side of the workspace.

Auto Explode tool 3. A quick way to get started is to Auto Explode the assembly. Click the Auto Explode tool on the Assembly tool bar, or use the Tools menu and select Auto Explode Assembly (figure 1).

figure
Figure 1. An example of an automatically exploded assembly.

This feature works well with most assemblies; however, certain constraints prevent an assembly from automatically exploding. In this case you must manually explode the assembly.

4. You can now fine-tune the view.

Expand Explosion tool a. To increase the separation between the parts, click the Expand Explosion tool.

Contract Explosion tool b. To decrease the separation between the parts, click the Contract Explosion tool.

Manual Explode Mode tool 5. To further refine the exploded view, move the parts individually. To move individual parts, click the Manual Explode Mode tool. You are now in Manual Explode mode.

    a. Select any planar face on a part that you would like to move. A set of directional arrows will appear where you click the part (figure 2).

figure
Figure 2. Directional arrows assist when manually positioning parts in an exploded view.

    b. Select any of the arrows to move the part in that direction. The active arrow turns yellow and the other arrows remain blue.

    c. Select any non-planar face on the part and drag, it moves parallel to the direction of the arrow.

    d. Select the other arrows to change the direction of movement.

    e. Repeat this process for all the parts until the exploded view is as desired (figure 3).

Exploded View Trail tool Note: Each time you move a part, the Exploded View Trail shows you the sequence of segments used to move the part. To hide the trail, toggle the Exploded View Trail tool or deselect the Exploded View Trail option on the View menu.

figure
Figure 3. A completed exploded view created by automatically exploding the view, then refining it manually.

6. When the Exploded View is complete, right-click the active Exploded View in the Design Explorer and select Exit Exploded View. You can also exit using the Edit menu. When not in Exploded View mode, your assembly appears in its original constrained state.

Note: To rename your Exploded view, right-click the name in the Design Explorer and select Rename.

7. Save the assembly.

Create a 2D Drawing Using an Exploded View
1. To start a new drawing, select File / New / Drawing. In the New Sheet Properties dialog box, select a template for your drawing and click OK.

2. If the Fill In Text dialog box appears, enter the information if desired and click OK to continue.

3. If no part or assembly workspaces are open, the Insert Design dialog box appears. Select an assembly with an exploded view to insert into your drawing.

4. In the Standard Views Creation dialog box, select the views that you want to insert into your drawing (figure 4).

figure
Figure 4. Use the Standard Views Creation dialog box to select the views for your drawing.

    a. Select an Exploded View from the Exploded Views drop-down list. The selected Exploded View will appear in the preview pane of the front view.

    b. As with any standard view, you can use the arrows next to the preview pane to change the orientation of the front view.

    c. Select the views that you want to insert into your drawing and click OK.

    d. Click the drawing sheet to place the view(s) (figure 5).

    Note: You don't have to worry if the view is too big or too small; you can change the scale after you have placed it on the drawing.

figure
Figure 5. Initially the view is inserted with a 1/1 scale.

5. To change the scale, right-click the view and select Scale from the pop-up menu. Use the Scale dialog box to change the scale of the view. For this example the scale is changed to 1.0/15.0.

BOM tool 6. To insert callouts, you must first insert a BOM. Click the BOM tool on the Drawing toolbar; then click the drawing sheet where you want it to appear.

Callout tool 7. Select the Callout tool on the Drawing toolbar. The Callout Annotation dialog box appears.

8. To insert a callout, move your mouse pointer to an edge of the part to which you want to affix the callout. The part is highlighted in red to indicate that you can select it.

9. Click the part once; then click the drawing sheet where you want the callout to be placed; then click once more to position the callout.

10. Click Apply on the Callout Annotation dialog box. Repeat this process for each callout that you want to insert.

11. When you finish close the Callout Annotation dialog box.

Tip: To add more than one balloon callout, check "Do not show this dialog next time" in the Callout Annotation dialog box and close it. Select the Callout tool again. Now you can quickly insert callouts without selecting the Apply button between each insertion. When finished, click the Callout tool to exit that mode (figure 6).

12. Save your drawing.

figure
Figure 6. The final drawing is completed with BOM and balloon callouts.

Exploded views facilitate visualization of an assembly in both 3D and 2D space. Now that you can create exploded views and document them in drawings with a BOM and balloon callouts, use this technique with your next complex assembly.

Next month we'll explain how to back up and replace your critical data stored in the repositories. Until then, look for me as the Alibre Assistant online in Alibre Design.


About the Author: Michael Todd


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