Copieng property values from Excel into SLDASM

Hello all,

At work I have to put 6 values into the custom propertyes of several
assembly files. These files can have configurations, but the
properties stay the same within a file. I also have a list in Excel
which contains the values of each property for each file.

Now my question:

Does somebody have a utillity for reading property values from an
Excel file and put these into a SWX Assembly custom property?

Thanks in advance for your help,

JD

 

No real need for a utility, Jan, unless you just want one. What you do
is insert a new Design Table in the SLDASM file(s) you want to change,
then you can Copy/Paste from your Excel file to the Design Table in each
Assembly. Each custom property column HEADER must be preceded by $PRP@
just as you would normally do in a Design Table. The entries will show
up as Configuration Specific custom properties, so if you have more than
one assembly configuration you need to have a row of values for each
configuration.

BTW, you can also drive the part number that ends up in the BOM this way
by inserting $PARTNUMBER as a column header with the desired value for
each configuration. It's does the same thing as right-clicking on the
configuration name (in the Configuration Manager tab) and selecting
"User Specified Name" under "Part number displayed when used in a bill
of materials".

Further BTW, I note that sometimes either Excel or SolidWorks (don't
know which) refuses to permanently accept the changes made to the Design
Table. The workaround in to open Excel independently first (open your
template file with your custom properties in it), then right-click on
your SolidWorks file's Design Table and choose "Edit Table in Separate
Window". You'll then have both windows open in Excel and you can
Copy/Paste from one to the other.

'Spork'

 

Jan,
If you still think you'd like to have a utility to do this, I'd be happy to
make one for you.
--Brenda

 

I've pasted in the text from a thread on another discussion group that looks
like what you want to do. You might get ahold of Stuart to see where he
went with this one.

WT
Yes that's what I'm trying to do, I made significant progress last night,
(after I learnt a bit about importing object libraries) I can now read from
a cell in excel, yay! I was then going to use parts of dereks custom
properties macro to add the cell contents to the solidworks file, And then I
was hopefully going to get it to step through all the files populating them
correctly (provided they have their filenames are spelt correctly.

Here is my code:
Sub main()
Dim appxl As Excel.Application
Dim partno As String
Dim myobj As Object
Set myobj = GetObject("C:\Documents and Settings\Stuart
Young\MyDocuments\XTRA 2002\parts2.xls")
Workbooks.Open Filename:="C:\Documents and Settings\Stuart
Young\MyDocuments\XTRA 2002\parts2.xls"
Cells(2, 2).Select
Selection.Copy
Workbooks.Add
Cells(1, 1).Select
ActiveSheet.Paste
ActiveWorkbook.SaveAs Filename:="C:\Documents and Settings\Stuart
Young\MyDocuments\XTRA 2002\testfile.xls"
ActiveWorkbook.Close 'close books
ActiveWorkbook.Close
End Sub

Any guidance would be appreciated

Stuart Young

Design Engineer,

****************************************

Gelârt International Ltd/ Medix 21 Ltd
Box 54117 Mana Paremata
Wellington New Zealand

http://www.gelart.co.nz/
mailto:
tel +64 4 233 0925
fax +64 4 233 0982

****************************************

-----Original Message-----

From: [mailto:]
Sent: Thursday, September 04, 2003 4:21 AM
To:
Subject: RE: [CAD] API tips

What exactly are you trying to do? What I am seeing is that you want excel
to populate your custom properties with data from the cells? If so, yes it
can be done and I will show you what I'm thinking if that is the case. If it
is, let me know which version of SolidWorks your wanting to do this with
(2001Plus, 2003, 2004??).

John

-----Original Message-----

From: Stuart Young [mailto:]
Sent: Tuesday, September 02, 2003 5:18 PM
To:
Subject: RE: [CAD] API tips

Can anyone guide me on how to import data from Excel into a solid works
macro so that I could then write it into the custom properties using a
derivative of Derek's macro? Something along the line of

Open excellfile. "C:\partdata.xls"
Cells (1, 1).select
Part number = selection
Cells (1,2).select
Description = selection
Cells (1,3).select
Cost = selection
Etc.....

Can this be done? Code that works in Excel macros doesn't appear to be
recognized in solidworks macros, Are they slightly different languages?

Cheers
Stuart Young
Design Engineer,

****************************************

 

Make sure you quit excel. I noticed that in the Task Manager that you can
end up with 8 or so instances of excel that are all hidden.

appxl.Quit