SOLIDWORKS Electrical 3D - Exercise 3

In this exercise, you use the 3D model data to create 2D views that you insert into a drawing. You then create a project drawing.

If you have not completed the previous exercises, download the Exercise 2 electrical project, unzip it to a local drive, then unarchive it.

Creating 2D Views

  1. Open the cabinet project in SOLIDWORKS Electrical 3D.
  2. On the SOLIDWORKS Electrical 3D tab of the CommandManager, click Create 2D Drawing .
    A 2D drawing file opens in the graphics area. The software uses the dimensions of the title block settings in the Electrical project configuration.

  3. From the View Palette Task Pane, drag the Front drawing view and click to position it on the drawing sheet as shown in the video.
  4. Click Insert > Tables > Bill of Materials.

    SOLIDWORKS manages the BOM. It is a bill of parts and not an equipment report, such as you might have in SOLIDWORKS Electrical Schematic. You use this SOLIDWORKS BOM mainly to meet mechanical drawing requirements.

  5. In the PropertyManager:
    1. Select the drawing view.
    2. Under Table Template, select bom-standard.
    3. Under BOM Type, click Top-level only.
    4. Click .
  6. Drag the BOM and click to position it below the drawing view.
  7. Use the hover over tools to modify the BOM:
    • Delete the Material column.
    • Use the column property edit tools for the Part number column to display the manufacturer part.
    • Add the Manufacturer column.

  8. On the Annotation tab of the CommandManager, click Auto Balloon and click the drawing view to automatically place the balloons.
  9. In the PropertyManager:
    1. Under Balloon Layout, click Layout Balloons to Top and clear Ignore multiple instances.
    2. Click .
  10. Verify that the balloon numbers match the items in the BOM.

  11. From the View Palette Task Pane, drag the Back drawing view and click to position it on the drawing sheet as shown in the video.

    Make sure that there is space below it for a hole table. To fill in the hole table correctly, you hide the door components.

  12. In the graphics area, select the drawing view.
  13. In the PropertyManager, under Save View as, click More Properties.
  14. In the Drawing View Properties dialog box, on the Hide/Show Components tab, select the three holes in the drawing view that you inserted, then click OK and to close the dialog box and PropertyManager.
  15. Click Insert > Tables > Hole Table.
  16. In the PropertyManager:
    1. Under Datum, for Origin, in the drawing view, select the lower-left vertex of the cabinet.
    2. Under Holes, for Edges/Faces, in the drawing view, select the three holes.
    3. Click .
    4. Drag to position the hole table on the drawing sheet and click to place it.

Creating a Project Drawing

You generate a project drawing from a 2D drawing. This process automatically adds a title block and saves the file in .EWG format in the Drawings directory of the electrical project.

To create a project drawing:

  1. In the drawing that you created, click Tools > SOLIDWORKS Electrical > Create Project Drawing .

    The system informs you that it created the project drawing and added it to the project.

  2. In the SOLIDWORKS Electrical Task Pane, right-click Cabinet and select Preview.

    A preview of the project drawing appears.