I've been trying to decypher this SolidWorks Help for a while and I guess I just don't understand. In this: http://help.solidworks.com/2010/English/SolidWorks/sldworks/LegacyHelp/Sldworks/drawings/Linking_Notes_to_Document_Properties.htm, it says:
"To automatically insert information in a drawing, you can link note text in the drawing sheet or drawing sheet format to document properties. For the procedure to add a link in a note, see Link to Property.
All SolidWorks documents have system-defined properties, including the following:
Property Name | Value |
SW-Author | Author field in Summary Information dialog box |
...and it goes on for quite a few items including dates and material. The only property links that work for me are file name and folder name everything else I've always had to enter manually. As we get busier it would be nice to have this working.
I haven't been able to figure out where to add information for "checked by", "eng approval", "material", "finish" etc. Even though I put the material on the solid or the design journal it just doesn't show up automatically. AND even though it's suposed to return "ERROR" if the information isn't found the only thing that does is "weight" and "scale"(I think). I assume the links have to refer someplace for the information but where? The "properties" of the Anotations in the Title Block are set to use custom properties from "current document" but it doesn't seem to make any difference how it's set. Am I suposed to create an Database or something in the drawing folder attached to the drawing, or model, somehow, for a reference? Just stabbing in the dark since at this oint I'm lost...
jw
Hi Gerald,
seems like you're a bit confused, but that's ok. This is very easy to understand.
Basically when you want to link some sort of information onto a drawing/annotation, solidworks deals with property values (properties).
File Properties/ CustomProperties are values stored within the document file that contain specific and custom information about itself.
There are generally two types of Properties:
1 - system-defined (SW-File Name, SW-Folder Name, etc,etc) - These are the fixed properties that are read-only
2 - Custom Properties...These are the actual Custom Properties, that you can edit, and tweak around for your own special needs.
If you point to File--> Properties (from a sldprt file)...you'll get the summary information windows pop-up.
There are three tabs here
As for the custom tab, these are also reffered to as the document properties (think of it as properties that don't rely on the configuration, while the configuration specific tab does.
So, if you want to link something onto a drawing for example, let's say, the date the document was last saved....With your drawing open, point to Insert->Annotations-->Note, now before you set the note on the drawing, on the left side you'll see the Note PropertyManager, under Text Format, right below the angle, there is an option called "LinkToProperty", select this option, and you'll have a series of option to chose from...
So now if you just select current document. You will see a long list of properties already available (these are all the system-defined properties we mentioned previously), pick "SW-Last Saved Date(Last Saved Date)" from the list and leave all other option default, click ok...and the note is ready to drop.
This is how you link a note to a custom property/file property....
Now, what we just did, is exactly the same as adding a new note, and instead of clicking on the PropertyLink tool, we type in the code...$PRP:"SW-Last Saved Date(Last Saved Date) straight into the typing box. This creates a link to the system-defined property Last Saved Date. If you hover over a linked custom property, once inserted, solidworks will show you the "code" that builds that link.
One thing good to know here, is the way the "code" works....basically, first you call, the type of property you want...in this case we just wanted the standard document (right from the drawing, because we want to know when it was last saved) property, for wich we use the "code" $PRP, the we separate this with a colon, and add the name of the property to retreive in double quotes ( " ). So again, $PRP (for the current document, in this case the drawing), then "SW-Last Saved Date(Last Saved Date)". There are 4 types of calls you can make (these are basically the 4 opions we had before, when using the link utility)...
Ok, so with all that said, if say you needed a field on your title block, with the name of the project the drawing was associated with, you would add a custom property to the custom tab under File->Properties, just name it "Project", and give it a value of whatever you like, say "Solidworks". Now you can do the same we did with the date, only for the custom property name you would use "Project", so if you were to type it, it would be like so: $PRP:"Project"
I hope, this helps...wow that was a long post...didn't mean to get carried away...
cheers