"Weight" in title block? 3

[MMike1]

I've done a search and didn't really find what I was looking for.

I'm trying to customize a sheet format. I have been able to get almost all of the fields I was by typing in, $PRP:"SW-whatever"

But weight seems to be different. I was looking at one of the other sheets and the weight field has:

WEIGHT: $PRP:"Weight"$PRPSHEET:"Weight"

But when I type it in, the "" around the last Weight, turn into { }....and the code doesn't work.

What's up with that?

And what's the diff between $PRP and $PRPSHEET?

Thanks

 

[Heckdogg]

My border has the following for weight:

$PRPSHEET:{WEIGHT}

and everything works fine. Have you tried to insert a part and create a custom link to the property and then save the sheet format?

 

[CorBlimeyLimey]

$PRP = properties drawn from SW defaults of a component.
$PRPSHEET = properties drawn from the Custom Properties of a component.

Use the Link to property in the Property manager section to link propeties to notes ... simply typing the "code" for the link does not work.


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[ctopher]

CBL has good advice.

Also, my .02, per drafting stds, weight does not belong in title block, it should be in a note.

Chris
Sr. Mechanical Designer, CAD
SolidWorks 05 SP1.1 / PDMWorks 05
ctopher's home site

 

[MMike1]

I'm trying to do what CBL said. And I'm there.... but it won't let me add weight to my list of properties. The "ADD" button is under-intensified....

 

[Heckdogg]

MMike1, add it to the custom properties at the part/assembly level, and then insert the part/assembly into the drawing.

 

[MMike1]

That's what I'm doing for specific parts. But I'm trying to make my generic drawing border "smart". My part number appears in the title block. I want the weight to appear as well. All I have right now is the word "weight".

When I'm linking the custom property to the text, I have the NAME of the property, (ie: "weight") then below I have the value. Do I type the $PRP code as the value?

 

[Heckdogg]

yes, or highlight the value and hit the "Link to Property" button and select the weight property.

 

[CorBlimeyLimey]

Link to Property
You can link the value of a document property, a custom property, or a configuration specific property to the text of a note. If the value of the property changes, the note text changes automatically.

To link a note to a property:

In the Note PropertyManager, click Link to Property

- or -

In the Note Properties dialog box, click Link to Property .

Select the place to link from:

Current document

Model in view to which the annotation is attached (drawings only)

Model in view specified in sheet properties (drawings only)

Component to which the annotation is attached (in assembly documents and assembly drawing documents)

View the list of available properties, which depends on your selection in step 2 and where the note is created.

Part or assembly document. The list includes the properties of the model document, including any custom defined properties.

Drawing sheet or sheet format. The list includes the properties of the drawing document, including any custom defined properties.

Drawing view. The list includes the properties of the model document shown in the view. (If a view is selected when you insert the note, or if the note is attached to the model in a view, the note belongs to the view.)

NOTE: All documents have system-defined properties. Drawings have system-defined properties that you can use to customize a sheet format. For more information on document properties in notes, see Linking Notes to Document Properties

To add a new custom property, or to edit an existing one, click File Properties, then edit the properties on the Summary Information – Custom and Configuration specific tabs.

Select a system-defined or custom property from the list, and click OK.

The Note text shown in the dialog box is the name of the property in the form $PRP:"<property name>". In the document, the note text is the value assigned to the property.

Prefixes for custom properties linked in notes are used as follows:

Prefix
Evaluated from:

$PRP:
Current document

$PRPSHEET:
Model in the view specified in Sheet Properties.

If the model specified in Sheet Properties for custom properties is Default, then for notes belonging to drawing views, the model in the drawing view to which the note belongs is used.

For sheet and sheet format notes, the first view in the FeatureManager design tree is used.

If a view is selected, the model for that view is used for all cases.

$PRPVIEW:
Model in the drawing view to which the note belongs

$PRPMODEL:
Component to which the annotation is attached


Links to dimensions are evaluated from the active document.

If the appropriate document for custom properties cannot be located according to the designations above, the following rules apply:

In edit sheet mode, all sheet format notes are blank. All sheet and drawing view notes show their property names.

In edit sheet format mode, all sheet format notes show their property names.

NOTE: When a note in a drawing is linked to a custom property or a dimension and then the property or dimension is deleted, the note displays ERROR!<variable name>. The parametric text is retained, and you can double-click the note to see the text. As soon as the property or dimension is available, the note updates to the correct value. Other items in the note are not affected.

You can choose whether to display the link error. Select or clear View, Show Annotation Link Errors.

NOTE: If a missing property or dimension is detected when opening a drawing yet to be saved in SolidWorks 2001Plus SP01 or later, a message asks if you want to break the link. If you choose to break the link, SolidWorks replaces the parametric text with the last known value. If no value is available and the note contains no other text, the note is deleted. The message appears only once.

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[MMike1]

Well I must be retarded or something. Because none of this is working.

I'm usually pretty good at this kind of stuff.

 

[ctopher]

well...you do stutter MMike1 (just kidding)
Is there a way you can send a screen-print of what you have?

Chris
Sr. Mechanical Designer, CAD
SolidWorks 05 SP1.1 / PDMWorks 05
ctopher's home site

 

[MMike1]

HOLY CRAP!!! I GOT IT!

It would seem that I AM in fact retarded....and I'd rather not publish what it was that I was doing wrong...sufficed to say...I should be kicked in the nads.

Thanks to everyone for their help!

(As we are JUST implementing SW here at work...and we're only two engineers... AND it was my bright idea to do this... AND therefore I'm going to be my own VAR... I'm sure I'll be here quite a bit.

Oh how I love internet forums......

(BTW can you post pics and stuff here?

and all that. I spend altogether too much time on another mountain bike forum and you can attach files and links and all that good stuff....)

Word to your respective mothers!

 

[ctopher]

good for you.
Click on Process TGML next to Emotions/Smileys, it explains.
good luck

Chris
Sr. Mechanical Designer, CAD
SolidWorks 05 SP1.1 / PDMWorks 05
ctopher's home site