I have the Header row in my BOM setup to automatically display the part number and title for the assembly. The problem I have is that as far as I know you can only link it to the model specified in the sheet properties, so if I have two small assemblies on the same sheet then both BOMs will display the properties in the header from whichever assembly is selected in the sheet properties. Is there any way to link these values to the assembly that the BOM is attached?
Hunter,
Did that work for you?
Sorry for the delayed response. I got backed up at work, and didn't have the time to investigate. The problem I'm having is it does not allow me to select "Component to which the annotation is attached" If I try to link it through the menu's it doesn't display anything, and if I try to type the command to link it manually it won't link it will just display the text I typed. This is why I currently have it set to Model in view specified in sheet properties.
To get the assembly properties into the BOM title, follow these steps. This works in SW2014:
1. Insert a projected drawing view off the view which defines the BOM. Position it off the side of the drawing sheet so that it doesn't print.
2. In the new view, insert a balloon on a component of the assembly. Change the outline to None and the text to Custom Properties. Select a custom property from the dropdown.
3. Double-click the balloon to edit the text. Change $PRPMODEL to $PRPVIEW to get properties from the assembly instead of the component.
4. Further edit the balloon text to generate the text with assembly properties as desired.
5. Double click in the BOM title to edit it. Place the cursor, and then click on the balloon to quote it into the title.
C
I have struggled for some time with finding an elegant solution to this problem.
Ideally, I'd like to place a parametric note in our BOM template but this does not work.
In the end, this is the method we use:
$PRPSHEET:"PartNumber": REV:$PRPSHEET:"Revision", $PRPSHEET:"Description"
As the original poster noted, this $PRPSHEET only gets you the properties for the assembly in the view specified in the sheet properties. If you have more than one assembly and BOM on a drawing, the other assembly's properties are not easily accessible from its BOM.
It is possible to save the BOM template with the $PRPSHEET:"PartNumber": REV:$PRPSHEET:"Revision", $PRPSHEET:"Description" in the header, so that you don't have to copy and paste it each time. Our template has LIST OF MATERIALS FOR $PRPSHEET:"PartNo"-$PRPSHEET:"Number". We're on SW2014 SP3.0.
Welcome to the forum. I suspect that when you set up your BOM, and linked the text in your header, in the "Link to Property" dialog box you made your selection with "Model in view specified in sheet properties" selected. If so, try selecting "Component to which the annotation is attached" instead.