Spotlight on Features: Why one of the assembly drawing view component does not update when I change configurations?

You create an assembly with some configured parts, in this assembly you also create some parts in the context of the assembly.

So far there is nothing wrong with this work flow. However, the problem arises when you want to create drawing views with different assembly configurations.

Assume a component –named square — has three configurations: 50 mm, 75 mm and 100 mm per side (Fig. 1)

The pin component has been created in the context of the assembly with a 20 mm reference dimension to the square component side (Fig. 2)

The assembly has also three configurations corresponding to each “square” component configuration.
Notice when the assembly changes configurations, the pin component updates such that its edge is always 20 mm away from the square component edge (Fig. 3)

You have a drawing where all the drawing views are displaying the 50 mm configuration (Fig. 4)

However, you want one of the views to display the 100 mm configuration. You click on the isometric view and
change the view reference configuration from the 50 mm to the 100 mm (Fig. 5)

After changing the configuration the “square” body updates to the 100 mm configuration, but the pin does not update (Fig. 6)

You open the assembly to check what is going on and now the pin updates.
However, all the other drawing views also update showing the square component in the 100 mm configuration. Is this normal?

The answer is yes. An in-context part, just as the pin in the current example, can only exists in one state. That is, it can only appear in the drawing in one size, regardless of the referencing part size. Also, when the in-context part updates it must do so in all the views.

If you must display different drawing views with different sizes, a better approach would be to create the pin component using also three configurations.
Therefore, when a drawing view requires to display the assembly using the 100 mm configuration, the “square” body will be at the 100 mm configuration, and the pin will also be at a configuration appropriately sized for the needed configuration.

Customer Service Subscribers can download the SOLIDWORKS files from the images from Solution Id: S-068715.

Mario Iocco

Mario Iocco

Sr. Technical Customer Support Engineer, SolidWorks, Americas.
Mario Iocco is a veteran CAD user. He started as a Mechanical Engineer first working in 2D with AutoCAD, moving on to 3D using  both SW and some  of the other CAD software on the market. He began his career with SolidWorks over 15 years ago. He started in R&D working on many of the new functionalities developed at the time -eDrawings, Sheet Metal, Weldments, etc. In the last few years, he moved to TS., working closely with VARs, Mario wrote the sheet metal functionality best practice manual, as well as creating hundreds of Sheet Metal Knowledge Base articles. He has presented webinars  on "Sheet Metal Tips and Tricks" and "Sheet Metal Bend Tables".