"THE HARDER WAY" (not as easy, but functional )

You can access the custom properties of any SolidWorks file by any of the following steps:

• Using the SolidWorks menus FILE à PROPERTIES
• In the configuration manager,  RMB (Right Mouse Button) on the configuration and choose properties
• RMB on the file in windows explorer and choose properties

You will see a dialog box called "Summary Info"

For part files and assembly files, the Summary Info dialog has three sections to it accessed by the three tabs at the top: Summary, Custom, Configuration Specific. Drawings cannot be saved with different configurations, so only Summary and Custom properties can be assigned to drawing files.

There are a couple ways to get your properties into your file.  Lets look at what I call "The Manual Way".  After "The Manual Way," I will go over a technique to place more than one property at a time, and follow the same properties every time with the option to add more at anytime.

Summary Info Tab

Summary Properties are simply text boxes that you can store useful information. Author, Keywords, Comments, Title, and Subject can take any text you feel like typing in.  Nothing has to be in this tab ever.  It is just for your info, nothing else.

Custom and Configuration Specific

Custom Properties exist in all three file types: parts, assemblies, and drawings. They are a huge power in SolidWorks. Custom Properties can contain more than just text. When creating a custom property you have to specify a Name and Value.

At the bottom of this dialog, is a list showing the current list of properties, their value, and their type. It also allows you to select an existing property, so you can Modify or Delete it. If you are modifying the value of a property, don't forget to press the Modify Button before pressing the OK Button.  I've made this mistake numerous times.

The Configuration Specific Properties operate in exactly the same way as Custom Properties. As you change the current configuration of you part or assembly, only the properties created for the current configuration will be shown. In contrast, Custom Properties will always be available regardless of the current configuration. For more information on creating and using configuration, refer to the SolidWorks Help.

To add custom properties:

1. Click File, Properties.

2. To add properties to the file, click the Custom tab. (To add properties to the active configuration, click the Configuration Specific tab.)

3. Enter a Name for the property, or choose a name from the list.

4.  Select the Type of value (text, number, and so on) for the custom property. 

5.  Enter a Value for the custom property that is compatible with the selection in the Type box.

6.  Press TAB to finiallize the property. The Properties box displays the name, value, and type of the custom properties.

Delete a custom property:

In the Properties box, click the Name of the property that you want to delete, then click the Delete Button or press the Delete button on keyboard.

Modify a custom properties:

1. In the Properties box, click the Name of the property that you want to change.

2. Edit the Type or Value as needed.

3. Press TAB

"THE EASY WAY"
This next technique I call "The Easy Way" involves an Excel template and the use of the design table.

To insert a Design Table: Choose the Insert pull down and choose Design Table

Source

Blank
Auto-Create
From File

Blank - Inserts a blank Design Table into the part or Assy with a line set for First Instance. This should be changed to Default to match what would be in your model already by SolidWorks default.

Auto-Create - Transverses through your configs and finds all the differences between each config (properties, mates, features, dims, colors, etc) and places them all in an Excel table in your SolidWorks part or assembly.

From File - Uses an Excel file from your network or Local drive to insert into your SolidWorks part or Assembly. This file should contain all your company properties, (description, part number for BOM, part number for drawing, material, drawn by, drawn by date, etc)

Link to file - (Option) It links bi-directionally to the excel file. I cant find a reason to use this. It makes a link to the file outside and creates a need to maintain a set of files that if lost could cause problems for your part or Assembly in the future.

Edit Control

Allow model edits to update the design table.
This option is an option I will not use. It allows models to be changed and updated from the part or assembly model. My belief is that if I put something in the Design Table I want it to be controled by the table. My thoughts, say you had a tabulated drawing. The drawing would have a tabulation on the face of the drawing, and the dims being controled by the tabulation would be called out as a letter on the drawing matching the letter on the tabulation. You wouldn't change the letter th change the tabluation, you would change the tabulation or add to the tabualtion to change the part or assembly. With that said lets look at the next option

Block model edits that would update the design table.
This option has the Design Table control the model. Just like a tabulated drawing. The tabulation controls the values of each configuration or version of the part or assembly. This option should be used.

Options

Add new rows/columns in the design table for:

New Parameters: If this option is selected, then SolidWorks when the Design Table is opened will ask you to add any new parameters (properties) to the DT (Design Table) (As seen in the Dialog shown "Add Rows and Columns"

In this Dialog choose what you whould like added to the DT and choose OK.
My thoughts on this is to just have this option unchecked. Then you as an user can add what you want, when you want when I open the DT. Unchecked is also easier to control the file if more then one person may work on this file or someone does a revision later and the dialog comes up and their not sure if they should add it or not.

Options (cont)

Add new rows/columns in the design table for:

New Configurations: If this option is selected, then SolidWorks when the Design Table is opened will ask you to add any new configurations, that were manually added to the part or assembly, to the DT (Design Table) (As seen in the Dialog)

In this Dialog choose what you whould like added to the DT and choose OK.
My thoughts on this is to just have this option unchecked. Then you as an user can add what you want, when you want when I open the DT. Unchecked is also easier to control the file if more then one person may work on this file or someone does a revision later and the dialog comes up and their not sure if they should add it or not.

You can add any property you like to your model (description, part number, material, etc) by using an easy little command "$PRP@property name"

Its broke down like this:
Along the top line of column B of the Excel based DT if you created the DT yourself from a blank Excel file and used "From File". Or the 2nd line starting in column B if you chose "Blank" from the Insert --> Design Table. Type $prp@ at the begining of any of the property that youwant to follow. The command $partnumber (notice no spaces) will set up the bill of materials when this file is used in an assy. Also as in this example the description will come out on BOM also. For the full set of DT parameters, in the SolidWorks Help, search for Design Table and on most of the help pages for it there is a link to Summary of Design Table Parameters.

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