Save time detailing bodies in SOLIDWORKS with Relative To Model view!

So you’ve got a multibody part, such as a weldment or other non-welded design (doesn’t even need to use Weldment tools) in SOLIDWORKS, and it’s time to detail each body as it would appear before being welded or assembled.  With assemblies, common practice is to detail each component part in its own drawing view.  But when all of the bits and pieces are contained in the same part (hence the term “multibody”), then we need another solution.  There are several, such as hiding bodies in View Properties, or creating Display States in the model (to be later selected in the drawing view properties).  But perhaps the simplest, easiest, and most user-friendly method for multibody parts is the Relative To Model view, otherwise known as Relative view.

Before you begin, you’ll need a multibody part, and a drawing in which to detail the bodies.

How it works:

1. Open the part (this can simplify the workflow) and the drawing.
2. From the drawing, Insert > Drawing View > Relative To Model > choose the model when prompted, or follow the instructions in yellow.
   

   Create a Relative View

3. Switch to the model if not already there (Ctrl+Tab is great for switching back and forth).  Notice that the left taskpane is activated (that’s due to the Relative To Model command) to show what is perhaps the coolest part: how you want the body to be oriented on the sheet!
   

   The left taskpane is ready for selections to orient the piece as it would appear on the drawing

4. Select the body(s) you want in the view, and pick faces or planes that define which side is up, or front, etc.  Let’s say I want the cross-bracing to be horizontal on the sheet.  I’ll make selections for front and top (blue and pink, respectively) and click OK.  This takes me back to the drawing.
   

   The colour tags are used to track which body(s) to include in the view, and which entities define the orientation

5. Click on the drawing sheet to place the view.  Et voila!  It should appear exactly per those face selections in the model.  Note that you can detail sub-weldments this way.  Most or all of the size information will be included in the Weldment Cut List table.
   

   Member shown with tangent edges hidden (of the rounded corners) and hidden lines visible (HVL) Display Style, in order to show the inner walls, denoting a hollow tube.  Alternately, can project a view that looks through the tube.

6. Marvel at how much time you could have saved, had you known about this sooner!

Attend our SOLIDWORKS Weldments LIVE Online training course to learn more multibody modeling techniques in SOLIDWORKS!