Tried F1, Google, my var etc..... :-P

In sheet templates, if I edit the template, I can reload the template sheet
in an old drawing and it updates the old drawing with the new template.

I have updated a part template with some new properties and can not get the
part file properties box to update in an old drawing. On a new part, the
updates are there.

I tried to use a macro, but the macro toolbar is greyed out, when in the
properties box.
How can I get these new properties in to old part drawings without having to
redraw the part(s)?

 

Are the property fields named the same in the old Drawing templates
(with $PRPSHEET: prefix) as in the Part files and do you have quotation
marks on both ends of the property also (in the Drawing template)? If
not, you simply Edit Sheet Format and change them or else you go back to
the old Custom Property names in the Part files for those parts. I get
the feeling this isn't what you're asking, but if it isn't then I don't
understand what you ARE asking. Do please clarify.

'Sporky'

 

Ok, this is what I want to do.

I have now added a new custom property, ( Number), to the Part template and
also changed the order of the list in the Part template, to make it easier
to enter the data.

I can make new part, insert the info, ( DrawnDate, DrawnBy, etc....) in the
part properties box, in the right order.

When I open an old part, I want the Custom properties box, to be the same as
the new Part template with the new custom property,( Number), in it and in
the same order as the new part template.

 

Ahh . . . that's better. OK, there are a number of ways to do this, but
none of them are COMPLETELY automatic. Semi-automatic is the best you
can hope for. There are a number of Custom Property applications around
that are either free or cheap, from VP apps to macros. do a Google
seach on the three keywords simultaneously: CUSTOM PROPERTY SOLIDWORKS.
You'll find applications like "Custom Propagator", "Change Custom
Properties", etc. Custom Propagator is a favorite of mine -- you can
change up to four Parts at a time with it without paying for and
registering it. Using these type applications you can add your "Number"
custom property to several or even many files at once. Another method
of changing the custom properties of a Part without opening the Custom
Properties dialog box is to include your chosen properties in a Design
Table. You insert a column header for each custom property, and the
name of the property must be preceded by "PRP@" (without the quotes) . .
.. all except the property for the part number that you want to appear in
a Bill Of Materials (BOM) for the Part in the next assembly Drawing.
THAT property must be simply $PARTNUMBER. You can create an Excel
spreadsheet with the additional properties (columns) you want to add to
all your old files and just cut and paste them into Design Tables in
those Part files you want to change. No, it's not automatic, but it's
not bad.

Mark 'Sporky' Stapleton
WaterMark Design, LLC
www.h2omarkdesign.com
Charlotte, NC

 

I'm kinda confused about what you're asking. By "sheet templates" do you
mean "document templates" or "sheet formats"? Sheet formats can be
reloaded, but templates of any kind cannot.

If what you are asking is to update the properties in a document using a
different template than the doc was created from, then the only way I know
of to do that is to use one of the macros that people have written for the
task. I don't think recording a macro will do it for you. A template is
just used to start a document is not linked to the

What these macros do is just copy doc props and custom props from one file
to another. There are a couple of them out there, but I can't steer you to
any off the top of my head.

matt