Inserting 2D Geometry into Pro/ENGINEER

by Angus Milne, Weatherford UK

This is a guide to inserting 2D data from another system such as SDRC® or AutoCAD® into Pro/ENGINEER. This 2D data can be used to produce a quick layout when multiple parts or assemblies do not exist in 3D Pro/ENGINEER format. This method can also be used to check compatibility of 3D geometry that may be required to work with existing tools.

1. Create a DXF file of the 2D part or assembly and save it to c:\temp or other folder location.

2. In Pro/ENGINEER Wildfire, create a new drawing. In the “new drawing” dialogue box, remove the “Default Model” and leave the box blank. Select any size and click OK.

3. From the dropdown menu, select Insert, Shared Data, From File and then navigate to your c:\temp or alternative folder. Select the DXF file saved there. A prompt will appear at the top of the screen: “Drawing is larger than format. Scale to fit format?” Select NO for a 1:1 layout. Another prompt will ask: “Move bottom left corner of drawing to screen origin?”. Select NO.

4. The 2D file will appear randomly on the created drawing. For simplicity, it is preferable to have the centerline of the 2D file located at the bottom left corner, i.e., 0, 0 in coordinates. To do this, select Edit, Transform, Translate from the dropdown menu. With your left mouse button, drag a box around the 2D object to highlight all the geometry, and press the middle mouse button to accept. In the Get Point menu, select Vertex and pick the vertex of the centerline with the geometry on the left-hand side. From the same menu, select Abs Coords. A command prompt will ask for a value for X and then for Y. Enter 0 for both. The position of the 2D file will look like that in Figure 1.

Figure 1.

5. Hide the drawing border by selecting File, Page Setup. In the “Page Setup” box, click on the format, uncheck the “Show Format” box, then click OK.

6. Save a copy of this drawing as a DXF file by selecting File, Save a Copy. Give the file a name and select DXF from the “Type” menu. Hit OK, and OK on the next prompt box.

7. Create a new part model using your normal procedures. From the top menu, select Insert, Shared Data, From File. Select the previously saved DXF file. Close the Information Window. In the “Choose Solid Options & Placement” box, with the Coordinate System set as default, hit OK.

8. The 2D file should look like Figure 2, with the centerline of the new part matching the centerline of the 2D geometry. You can now insert this part into an assembly like any other Pro/ENGINEER part.

Figure 2.

Angus Milne is a design engineer at Weatherford, located in Aberdeen, UK. He can be reached by email at Angus.milne@eu.weatherford.com.