This SOLIDWORKS PDM blog is the first in a three part series. The information about SOLIDWORKS drawing properties contained within is the foundation for the other two topics. The second post (Part II) will be about linking model properties to the drawing file data card. This blog post comes directly from a SOLIDWORKS knowledge base solution: S-010321. The last post (Part III) will also explore linking drawing or model properties to the file data card with a little bit of a twist. The details in the last post is the result of an experiment per a customer’s request.

Please note that this blog is not about how to link annotations/notes to specific properties, but rather highlight the fundamental differences between each type of property link. If you want to learn more about how to create property links, then go to the following webpage: help.solidworks.com.

What the heck is $PRP, $PRPSHEET, $PRPMODEL, and $PRPVIEW?

Upon reading this question, you might answer as a SOLIDWORKS user, “Sure, I know what these property links are, but what does this have to do with SOLIDWORKS PDM?” The answers to this question are clearly defined in the next two blogs. For now, realize that the specifics below are beneficial to both SOLIDWORKS users and SOLIDWORKS PDM administrators.

 

$PRP – Link to properties within the drawing file

Property link setting:

In SOLIDWORKS drawings, there are properties for the file itself and properties of the model/s contained within the drawing views. In this case, the link is established with the properties of the current drawing file. The property link referred to here is “Current document.”

See example figure below showing a SOLIDWORKS drawing file and the custom property created for it – “DocumentProperty.” The evaluated value for this custom property is “This is a document property.”

 DocumentProperty

In the next figure below, notice the “Description” in the title block. This annotation is linked to the file custom property named “DocumentProperty.” If you hover over the annotation in the sheet format, you will see the gray box appear showing “$PRP:’DocumentProperty.'” Another way to see the link property setting is to edit the sheet format, right mouse click on the annotation, and choose “Edit text in window” from context menu. This means that the value shown comes from a custom property within the SOLIDWORKS drawing file.

 This is a document property.

$PRPSHEET – Link to properties of the model for the chosen view in the sheet properties

Property link setting:

 Property Link Setting

In SOLIDWORKS drawings, you can setup sheet properties such as sheet name, scale, and type of projection (first angle or third angle). One of the settings is “Use custom property values from model shown in.” Basically select the view on the drawing where the notes/annotations pull the values from the model contained within. Think of the view like a “portal” to your model and the custom property values for it are shared with the notes/annotations on the drawing. The default value for this setting is to use the model properties from the first view inserted into the sheet. The property link referred to here is “Model in view specified in sheet properties.”

See example figure below. Notice how the “Description” property value from the SOLIDWORKS Ratchet part file is linked to the title block annotation in the SOLIDWORKS drawing. If you hover over the annotation in the sheet format, you will see the gray box appear showing “$PRPSHEET:’Description.’” Again, an alternate way of displaying the linked property is to edit the sheet format, right mouse click on the note, and choose “Edit text in window” from the context menu. This means that the value displayed comes from the model shown in the view selected under sheet properties. Hence the name of the link: “$PRPSHEET”.

 Model description

To access the sheet properties, right mouse click anywhere on the SOLIDWORKS drawing sheet (don’t mistakenly select a view) and choose “properties” from the context menu.

Sheet

The figure below shows the dialog that appears. Focus on the setting that pertains to “$PRPSHEET.” Please note each sheet in the drawing can have distinctly different settings.

Default

Another way to access the sheet properties is by going to the sheet name in the feature tree, right mouse clicking on the name, and choose “Properties”.

$PRPMODEL – Link to properties for a model component in a specific drawing view.

Property link setting:

Property Link Setting

This property link maps to a specific model component custom property value within an assembly. For example, the battery part shown in figure below has a series of custom properties associated with it. Notice the value for “sw_model_description.”

Property

The following figure below shows an exploded assembly view in a SolidWorks drawing. One of the model components of that assembly is an “AA battery.” A note was created and linked to a specific custom property for the battery component – “sw_model_description.”

AA battery

This type of property link is commonly seen in drawings with views showing part or all of an assembly. The note will point to a certain property value for one of the assembly parts displayed through the view.

$PRPVIEW – Link to properties for a model in a selected drawing view.

Property link setting:

Property Link Setting

This property link is very similar to $PRPSHEET. The main difference is the note/annotation maps to a model property in any viewon the SOLIDWORKS drawing. It seems logical why this property link is called $PRPVIEW. $PRPSHEET, on the other hand and as stated earlier, references property values in the model shown by the view defined within the sheet properties.

Please refer to the figure below. Notice the feature tree shows two separate views. On sheet one (not shown), there is a view of the exploded assembly. Sheet two-of-two also has a single view, but it displays a shaded view of just the battery pack subassembly (shown in figure). The battery pack assembly named “Base_” has a “Description” custom property with associated value. The value for the “Description” is “Battery pack for ACME cordless products.” Upon creating the view of the shaded battery pack, a note was inserted and linked to the property “Description” for the subassembly. Hovering over the note will cause a gray box to appear with the custom property name associated with $PRPVIEW. In this case, the gray box contains “$PRPVIEW:’Description” of Base_.’” Instead of hovering over the note, right mouse click on it and choose “Edit text in window.”

Exploded

Conclusion

For this post, the fundamental differences for $PRP, $PRPSHEET, $PRPMODEL, and $PRPVIEW linked properties have been explored in detail. Reading this has enabled you to better understand what they are and how they are applied to SOLIDWORKS PDM file data cards in Part II and Part III of this series. This blog was also written with the notion that it would benefit SOLIDWORKS users without SOLIDWORKS PDM.


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