Link drawing property to model property

[drillrig]

Hello all,

Is there a way to link a drawing custom property to a custom property in the part/assy? I can't seem to find the answer anywhere in this forum.

In the File-Properties-Custom tab the syntax I thought would work was $PRPSHEET:"TITLE1" where TITLE1 is the property in the part or assy. But this doesn't seem to work.

Thanks in advance!

- Chris

 

[CorBlimeyLimey]

See the last post (by EEnd) in thread559-138421

 

[drillrig]

Limey,

I looked at the post you referenced. The macro by EEnd is fine, but my property names are different and therefore it doesn't work. I'd rather not get into programming (which I can't do anyway!!!)

What I REALLY want to work is what Gildashard said in that post, but it doesn't seem to work for me.

Regards,

- Chris

 

[designer22]

Chris,

Which version of SW are you using.

2009 has a "Property Tab Builder" and you can create properties for Assembly,Part and Drawing.

If not you can create a text file with all the properties and point to that file in SW. These properties will be available in "Custom" tab.

Link these properties in your drawing.

Hope this works.

Thanks

 

[drillrig]

designer22,

I am on SW2009 SP2.1. I tinkered with the Property Tab Builder but it doesn't seem to be able to link a drawing custom property with a part/assy custom property. From all that I've read, the syntax:

$PRPSHEET:"custom property name"

is supposed to read the custom property name of the model displayed in the drawing. This works fine for notes and such, but not for a drawing custom property itself.

Regards,

- Chris

 

[TheTick]

$PRPSHEET:"{custom property name}" has always worked for me.

Remember that custom property names are case esensitive.

 

[CorBlimeyLimey]

drillrig,

Propagating the model custom properties to the drawing document's custom properties is different than propagating the model CP's to a note in a drawing.

It is easier than you think to modify EEnd's PropertySync macro to the property names you are using.

 

[designer22]

Chris,

I have few different custom properties liked to the part are working without any problem.

Please check the link
Can you please post the drawing file?

Thanks

 

[CorBlimeyLimey]

designer22,

No need for drillrig to post a file. The problem is not related to linking a note or annotation on the drawing. It is linking the drawing document properties itself.

Just open a new drawing, go to File > Propeties and try to populate a field in the Custom Properties section with a CP from the model.

 

[drillrig]

All,

I have attached a screenshot of my drawing properties. The model referenced by the drawing has its own custom property with the name:

TITLE1

But as you can see the software is not reading the custom property from the part file.

What am I doing wrong?????

Thanks again.

- Chris

 

[TheTick]

No screen shot of the model's properties?

 

[drillrig]

TheTick,

Here's a screen shot of the model properties.

Thanks.

- Chris

 

[TheTick]

What happens when you use the drawing's linked property in a note? Does it resolve then?

 

[drillrig]

Yes. In fact I have it linked in the title block. See this screenshot. When I mouseover the words you can see what it's linked to.

- Chris

 

[TheTick]

I would call that a success. Problem solved.

p.s. nice job w/ the screenshots, especially the last one.

 

[drillrig]

Well, not really.

It works fine for linking in the drawing title block, but not when linking in the drawing custom properties.

Any other thoughts?

- Chris

 

[TheTick]

The property is linked. It works when it is read. At least it is serving its purpose.

My drawings do the same thing. The evaluated value does not resolve in the properties dialog but it resolves in notes. I never really considered it a problem. Just used to it, I guess. Here we are all conditioned to linked properties effectively saying "see the model for the real value".

 

[CorBlimeyLimey]

drillrig,

What is the purpose of propagating the drawing CP's with the model CP's?

Although this has been requested several times, I have never really understood the need for doing such.

 

[CorBlimeyLimey]

Compare the attached macro with EEnd's macro to see the changes. Using the Edit > Replace function, it is very easy to change all instances of number to TITLE1 and description to TITLE2 ... and that's all that's required.

 

[drillrig]

Limey,

The answer to your question is best said by Stoker in the previous thread that you referenced...if I may quote:

"I can see the value in this, especially when a PDM system is being used. For example, if you are pulling the drawing number and description fields into the title block from the referenced part/assembly and you do not also have these custom properties in the drawing file, you will not have these properties available when looking at previews of the drawing or when searching through the PDM system. You will also not see the description show up when you highlight the drawing file in Windows Explorer, nor will you get the description in the windows status bar (both very useful). In my opinion, it is best to have the description field in both places - part and drawing, which is what is being requested."

Thank you very much for the macro. I will dig into it and see if I can get it to do what I want. I also found a macro from CustomSolids.com which has similar functionality.

My bottom line: Why do I need to run a macro to do this when using the $PRPSHEET syntax works just fine in drawing notes, title block, etc?

- Chris