How to Detail One Member of a Weldment Part
By Leslie Lougheed

When working with the Weldment functionality in SolidWorks, the Relative to Model View tool can add a view to the drawing of just one structural member.  A Relative to Model View is an orthographic view that is defined by two orthogonal faces/planes in the model.  It can be made of an entire assembly, part, or just a specific body(s).  This view is especially useful for a structural body member that has a profile that is not standard or is cut to a specific shape.  From the Relative to Model View, Projected Views, Section Views, Detail Views, etc. can be made to fully convey the geometry of that structural member. 

To make a Relative to Model View in a drawing, click Relative View on the Drawing toolbar, or from the pull down menus, Insert>Drawing View and select Relative to Model.  SolidWorks needs to know which file to place a Relative to Model View of.  This can be done in multiple ways:

1. Switch the window to the weldment part file using either control tab or the Window pull down menu.
2. Use File>Open to open the weldment part file.
3. Right click in the graphics area and select “Insert from File” to open the weldment part file.
4. If a view of the weldment part file already exists in the drawing, select that view.

Once the weldment part file is open in SolidWorks, the Relative View Property Manager is looking for some input.  The first thing to define is the scope of the relative view.  Is the view going to be of the “Entire Part” or just “Selected Bodies”?  Select the “Selected Bodies” option, and then select the body (or bodies if more than one body is needed in the view) from the graphics display that is desired for the Relative View. 

Then define the orientation of the new view.  There are many ways to define the view.  Two faces/planes need to be selected from the model, and then the drop downs specify the orientations of the selected faces/planes- Top, Front, Right, etc.   For example, select Front from the first pull down menu and select a face/plane to be oriented as the Front.  Then select Top from the second pull down menu and select a face/plane to be oriented as the top.  The first orientation face will be placed normal to the screen in the drawing view.  The second orientation will define the rotation of that face in the drawing view.

Once the orientations are defined, select the green check to confirm the input.  SolidWorks will then switch back to the draw and the Relative to Model View will be at the cursor.  A simple left click will then place the new view onto the sheet.  From here, Projected Views can be made from this view as well as Section, Detail Views. 

Keep in mind that the Relative to Model View is not just limited to weldment files.  It can be used on any part or assembly to help define a view that is not a standard view or that is not already established.