linked properties, BOM

[earlpatrick]

what i am trying to do is this;

i want a block that i can insert into a drawing that has a note with linked properties that reference the bill of materials. specifically i want to have the note reference the following columns in our BOM;

1. part number
2. part quantity
3. part classification (this is a custom property that we've set up)

i do not want the block to show the item number and i would prefer to have the item number column hidden in the excel file. basically, what it comes down to is that we need this information in an excel spreadsheet that we can transfer into our sequel database and item number is irrelevant. also, i want our assemblers to be able to look at an exploded assembly and follow the annotation leader and find the part number instead of an item number so that they don't even need to look at the BOM.

in addition i would love a list of custom & standard properties as they apply to annotations as opposed to the list in the help which refers only to the BOM and design tables as far as i can tell. $PRPVIEW: vs. $PRP: for example. in fact, a complete list of solidworks standard & custom properties period would be of great help.

thanks very much.

 

[SnowCrash]

You can create any custom or configuration specific properties (file/properties/summary-custom-configuration specific) you want and name them anything you want. The existing ones cover a lot of your needs. If you will use a custom property all the time, then include it in your template part.
Open a drawing for your new part. Insert a part view. Create a note and click to locate it on the sheet. Select "link to property" and then chose part or document., then the property you want to use. Click the checkbox to finish. Select the note and save as a block. Now you can insert this block into any drawing.
A block can of course feature multiple notes and lines. You could use a block or incorporate the notes into a template. It could be part of a drawing template or a format, depending on what you want. You will have to regen the note when you load the block to a new part.
I know this is not a complete description of the process, but it should get you started.

Crashj 'not a blockhead' Johnson

 

[earlpatrick]

thanks for the input. here is the answer i got from the solidworks api folks. it looks like the only way to really get what i want is to write it in code. does anyone know a good book on API for solidworks?

The following identifiers are available for the linked notes:
$PRP - Active document
$PRPMODEL - Selected component in view
$PRPVIEW - Document in view
$PRPSHEET - Document in sheet

From there, any custom property element in the specified document is
available.

The use of PRPMODEL is a very specialized identifier and is determined
by what the note is attached to. Once the note is converted into a
block, the connectivity is subsequently lost. Inserting the block back
into the document does not regain the connectivity that once existed.
Thus, the block shows the actual text of "$PRPMODEL:SW-File Name".

Given the description of the problem and what is currently being done.
The functionality of custom property linking and the block files will
not accomplish the desired task.

On the other hand, you can use the API to query the BOM on a drawing and
directly create the notes as desired. This will give you the control
over what exactly is required and what should be presented to the user.
The following will be a set of methods that will assist in the
construction of this functionality: View.GetBomTable - Obtain the BOM
BomTable.Attach3 - Activate the BOM BomTable.Get??? - Set of methods to
query data from the columns of the BOM BomTable.Detach - Deactivate the
BOM ModelDoc2.InsertNote - Create a note at a selected location, returns
the Note object Annotation & Note methods - Adjust any properties for
the note


Regards,
Earl Hasz
API Support Manager
SolidWorks Corporation earl patrick
epillsbury@bensonglobal.com

http://www.bensonglobal.com

 

[dogarila]

Check out thread559-20992, you may find some help there.

Andrew