Accessing Custom Properties of unopened SolidWorks models

Hi there,

I'm doing some tweaking of my custom property routines, and have the
following issue. I can modify the properties of a drawing easily
enough, but is there a way to access the properties of a model in a
view in a drawing without opening the model? I want to write a
description of the part in my drawing custom property description
field, and I'd like to get that description from the model's
description custom property. I can certainly do this by opening the
model, but this seems to be a rather un-elegant solution. One of the
issues is if the model is large this all becomes rather time consuming
and cumbersome.

I use the model custom property in the drawing to display the
description field using the $PRPSHEET functionality, but can't seem to
figure out if this can be accessed from VB.

Thanks in advance,

Chris

 

No, unfortunately, this isn't a general custom property. I'll keep
poking around to see if I can figure out a less cumbersome way of
doing this. I got it working by loading the model, but it's not what
I'd call an elegant solution.

Chris

 

Chris,

No, Robert is right.

You state you are using Custom Properties, in your part, and want the
Drawing to have the "same" Custom Property as the part in the drawing view.

If you are using $PRPSHEET to do what you want, then you are using a Custom
Property that can be accessed, read, and written using Microsofts DSOFILE
utility, which is available on the Internet.

If you right-click on the part your want in Explorer, you will see a Custom
tab, that will have your parts Custom Properties in it. If you are doing
something other than what is listed here, you need to be more specific,
other than saying "No, it isn't...."

Perhaps you are wanting to get a Configuration Specific property instead?


Mr. Pickles

 

I use the model custom property in the drawing to display the

By using VB, you can easily write a macro to get the selected model handle
and write custom properties. If the drawing is open, the model is loaded as
well in most cases, unless the drawing is a lightweight drawing or the
models are lightweight in an assembly. In a such case the model has to be
loaded to get the model handle. Refer to API help on custom properties.

Hope this was what you were wondering!

-h-

 

Absolutely. Thank you. I had the name of the file, then I used
GetOpenDocumentbyName to get a pointer to it that I could pass to
CustomInfo2 to get the custom property I wanted.

Trivial almost. Thank you very much for the suggestion.

The dsofile thing was not appropriate because I'm transitioning all my
custom properties to be configuration specific and dsofile doesn't let
you get at those.

Thanks to all who commented.

 

As you have discovered, SWX will not allow you to do anything with Config
Properties outside of SWX.
However, what you can do is launch SolidWorks invisibly, do the task and end
SolidWorks session. Have a look at "SolidWorks Visible or BackGround
Example" in SWX API Help.

--
Tony O'Hara
Melbourne, Australia.

Absolutely. Thank you. I had the name of the file, then I used
GetOpenDocumentbyName to get a pointer to it that I could pass to
CustomInfo2 to get the custom property I wanted.

Trivial almost. Thank you very much for the suggestion.

The dsofile thing was not appropriate because I'm transitioning all my
custom properties to be configuration specific and dsofile doesn't let
you get at those.

Thanks to all who commented.[/QUOTE]