How do I link information from .sldprt into drawings?

[Pat]

I'm pretty new to SW. I Would like the information that I put into
the properties tab of a solid part show up automatically in the title
block of a drawing file when a new drawing is created. ie. material,
finish, drawing number, etc. Is this possible? If it is, how do I
pull it off?

[David McCall]

Actually, this is pretty easy to do.

enter as a note on the sheet

$PRPSHEET:{x}

where x is the property that you want to show up on the drawing.

you can define any property you want by right clicking on the
configuration of the part in the configuration tab (third tab over from
left). The go to properties and click on custom.

I can send you a sample of the title block that we use if you want.

David

[Rob Campbell]

The correct syntax is '$PRPSHEET:"x"', not "$PRPSHEET:{x}". Other
than that, David's solution is correct. But he glossed over a detail
that you might not know, being new to SolidWorks. When you enter a
note in the form of '$PRPSHEET:"x"' (where x is the name of the
property), the value of x comes from the model specified in the sheet
property dialog. It defaults to the model in the first view inserted
in the sheet, which is the only model in most cases. If there are
views of multiple models, however, the default may not be what you
want. To override it, open the properties dialog for the current
sheet by right-clicking on the sheet name in the tree view and
selecting "Properties...". Select the view with the model whose
properties you want to use from the "Use custom property values from
model shown in" list box.

You do not need to remember or manually type the name of a property to
include it in a note. There is a "link to property" button in the
note dialog (or note property page, as of SW2001+). This brings up a
dialog that allows you to select from the list of properties defined
for the model and/or drawing. Note that the syntax is a little
different for properties taken from the drawing or the model:

$PRPSHEET:"model-property"
$PRP:"drawing-property"

When I first started using properties in notes, I did not realize that
you could include multiple links or links and other text in the same
note. Initially, for example, I had two separate notes to allow two
lines to be specified in the revision block:

'$PRP:"rev1-line1"'
'$PRP:"rev1-line2"'

Now I simply have:

'$PRP:"rev1-line1"
$PRP:"rev1-line2"'

(Notes are enclosed in apostrophes.)

Rob Campbell

[Pat]

Thanks Dave!
That worked great! It was exactly what I needed.

pa...@serraelectronics.com (Pat) wrote in message news:<b41c8cb7.02061...@posting.google.com>...

[Michael Rice]

"Rob Campbell" <rob.ca...@att.net> wrote in message
news:f9a77c9d.02061...@posting.google.com

> It defaults to the model in the first view inserted
> in the sheet, which is the only model in most cases. If there are
> views of multiple models, however, the default may not be what you
> want. To override it, open the properties dialog for the current
> sheet by right-clicking on the sheet name in the tree view and
> selecting "Properties...". Select the view with the model whose
> properties you want to use from the "Use custom property values from
> model shown in" list box.
>

I am running SWX 2001+ SP2.0 and the note defaults to the properties of
the view the note is attached to.

To take this one step farther, I created a block containing the
properties in my part file. However, I want to include the detail #
(SWX calls it an item # I think) and also the quantity required for one
assembly. These properties are automatically set up in the assmebly &
BOM, but can you access this same information in the detail drawing?

--
Posted via Mailgate.ORG Server - http://www.Mailgate.ORG

[kwbosch...@earthlink.net]

Michael,

Go here, and download the BOM/Note Linking Macro:

http://www.extremedp.com/extreme/monthlymacro/monthly%20macro_march.zip

Hope this helps,

Ken B.