Home » How to use alternate position view in SolidWorks?

There are a number of situations where it is useful to superimpose one view over another. This could be to show the difference of overall dimensions depending on if the equipment is open or closed. Otherwise it can show the maximum range of motion, either linear or angular. SolidWorks has a feature called “Alternate Position View” which makes this process very easy.

Open the assembly created for “How to make a subassembly flexible in SolidWorks?”. Select “Make Drawing from Assembly” from the file menu.

Place a front view and select “CYL RETRACTED” as the reference configuration. Use “Project View” to place the top and isometric views. If not automatically applied, set the reference configuration to “<link to parent>”.

An “Alternate Position View” will superimpose one or more configurations over the current configuration. They can be applied to any of the standard views. The superimposed configuration will appear as phantom lines, this is normally sufficient to differentiate it from the base view.

Select “Alternate Position View” from the View Layout” tab, then select the view to place it on. Selecting “New configuration” adds a new configuration and opens the assembly for editing. As a configuration already exists, it will be selected.

As the rack is quite small relative to the cylinder. Set the views to the shaded with edges display style, to differentiate the two. From this point, any relevant dimensions can be added to the drawing.

Ultimately, the number of alternate positions shown will depend on the design. Where the alternate positions cannot be clearly dimensioned, consider separating them onto separate views (e.g. multiple front views).

To edit an alternate position, expand the view in the design tree to reveal the desired alternate view. Right click and select “Properties, this opens the drawing view properties. From here the configuration can be changed.