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Manufacturing

A Few Simple Steps Turns Two Dimensions to Three

14 Dec, 2004 By: Michael Todd Cadalyst

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Use Alibre Design to Create 3D Solids from Existing AutoCAD 2D Drawings

Last month's Alibre Design Tech Tip focused on how to quickly and easily create fully documented auxiliary views based on a 3D model. This month, we focus on how to create a 3D model from an existing 2D drawing or sketch. Having a 3D model offers important benefits including visualization; accurate measurement of physical properties, such as weight and volume; and interference detection; to name a few. In production environments where 2D drawings are critical, a 3D model enables you to automatically make changes to the 2D drawing with one simple step instead of having to make multiple manual changes.

Converting a 2D AutoCAD File into a 3D Solid Model in Alibre Design
Converting a 2D drawing into 3D model often requires a few steps. In this example, we will create a part by importing a drawing in DWG format, then extruding and revolving sketches in the drawing to create a 3D parametric solid model.

• Click here to download the sample file, BASE-STAND.DWG (35kb).
• Import the AutoCAD file into Alibre Design. In the Home window, select File / Import (figure 1).

• Select DWG from the Files of Type pull-down list.
• Browse to the AutoCAD file, then select Open.
• The 2D drawing will load in a drawing window.

To create the base for the 3D model, you will use part of the imported drawing.

• Click the Select tool on the sketch toolbar to enter Select mode. This also activates the sketch.
• Press the Shift key and select the lines in the front view of the drawing to use as the sketch for the base feature in the 3D model. When selected, the lines are highlighted in blue (figure 2).

• Select Edit / Copy (or Ctrl+C) to copy the sketch to the Windows Clipboard.
• Open a new part workspace, select File / New / Part.
• Select the XY plane in the Design Explorer.
• Click Sketch / Activate Sketch.
• Ctrl+V to paste the sketch into the part workspace (figure 3).

• Click Feature / Boss / Extrude.
• Select Mid plane from the Type dropdown list.
• Enter 10, the value from the drawing, for the distance.

The feature is shown along the left side of the workspace in the Design Explorer as Extrusion 1, and is based on Sketch 1. To create the next feature, go back to the drawing to select additional sketch figures. Press the Shift key and select the lines in the drawing to use as the next profile. Select the lines highlighted in blue (figure 4).

• Select Edit / Copy (or Ctrl+C) to copy the sketch to the Windows Clipboard.
• Select Window / New Part (1) to return to the part workspace.
• Select the XY plane, then click Sketch / Activate Sketch and Ctrl+V to paste the sketch figures.

You will use a Revolve Boss to create the next feature. However, this command requires that the sketch be closed, so you will need to edit the lines to form a closed sketch (figure 5).

• Use the Line tool (figure 6) to add a line (a) as shown in figure 5.

Figure 6. The Line tool.

• Use the Trim tool (figure 7) to remove lines (b) and (c) as shown in figure 5.

Figure 7. The Trim tool.

Now your profile is clean (figure 8).

Note: You can also use the Analyze Sketch feature to check for gaps or overlapping lines in sketches.

• Now that the sketch is closed, click Feature / Boss / Revolve.
• Select the y-axis as the axis for the Revolve operation (figure 9).

Revolution 1 appears in the Design Explorer (figure 10).

Conclusion
Now that you have converted your drawing into a parametric 3D model, you can use this model in assemblies and new drawings. Any changes to the model will automatically be reflected in all those assemblies and 2D drawings. To convert your more complex drawing files into 3D models, continue to copy and paste sketch figures and use them to create additional 3D features.