Using the Configure Feature within Models and Assemblies

Many SOLIDWORKS customers use configurations as a great way of creating multiple versions of a part or an assembly within the same file, using this approach allows for quick generation of models to customer requirements.
There are a number of methods of creating a configuration with some being more time consuming than others, manual generation of a configuration can therefore take quite a while as each feature or part needs to be manually altered in each configuration. We can also use design tables to link the configurations to a excel spreadsheet. Another method (and the basis for this blog) is the use of Configuration tables to configure features or components, these can be accessed by selecting the feature required from the design tree, right clicking and selecting “Configure Feature




This will bring that feature up in a tabulated form with configurations on each row and the feature (and any associated options) as the columns (in the example below i have clicked on the down arrow next to crossbar extrude and checked the length box, this adds an additional column to the table and allows me to configure the length of extrusion for this feature (it has been renamed to something meaningful)


Click to select the extrude length into the table


This then allows easy configurations of multiple variants of the model, if the feature is to be suppressed in a particular configuration check the box, otherwise leave it clear to leave the feature unsuppressed (in this case we want this feature for all configurations so we will ignore it (we could right click and delete that column if required). New configurations can be generated by clicking the last row and giving it a name and adding the configured values into the table. This is a very quick way to work as it’s simply data entry and ticking boxes.


5 configurations added with various extruded lengths

With the table open we can double click dimensions from the graphics area) to add them into the table or click on features to add them to the table to allow further configuration of model dimensions or features.  In this example im going to add the height and width values for the crossbar from the crossbar sketch (allowing me to alter the timber size used for each crossbar) ive double clicked to add the crossbar sketch into the table then selected the two dimensions I wish to control from the dropdown for the 2000mm configuration ill change the height and width values to 60mm and 40mm respectively.



Crossbar profile height and width fields added in

At this point I would recommend giving any dimensions you wish to configure meaningful dimension names (double click on a dimension and changes its D# to something meaningful such as length or width, that way it’s easier to recognise what value is being controlled in the table

Saving the table
By default the table that you see on the screen is a virtual table, if you click ok it will create the configurations but you won’t be able to retrieve the table again as it never physically existed, the data will however have been applied to your model. If the table format is one that you wish to return to in the future you need to name the table and click save table.


Enter a name and save the table

Once this has been done you can return to the table as required to add or edit your configurations by accessing the table from the tables folder on the Configuration Manager tree.

Custom Properties
One of the issues people often have with configurations is that when they use a configured part or assembly it doesn’t correctly populate their Bill of Materials and the potential problems that may result from this. Using Configuration Table we can overcome this issue as we have additional button to add custom properties to our table, simply press the properties button to add a property and then check the box next to the required properties in the dropdown, you can now add the configuration specific information to the table and this will appear when that configuration is used within a BOM.


Press the hide/show custom properties to add properties fields to your table


This is my final configuration table, I’m changing the length of the crossbar, the profile dimensions for the crossbar, the material, whether it has mortices for the slats and the description, all from within the same table

Using different configurations of the same part in a BOM will now present different materials and description values for each configuration.


Resulting bill of materials entries for different configurations of the same part

Design Tables or Configuration Tables?
This is a difficult question to answer and personal preference comes into play, excel based design tables have the advantage of access to all of your usual excel functionality if you require things like equations etc. Personally I find the configuration tables nice and easy to use, clear checkboxes to suppress and unsuppress features, plus easy access to your list of custom properties etc makes the experience a little easier to figure out and work with.

Generally both have their own merits and certain models and workflows might lend themselves better to one approach or the other and as with everything SOLIDWORKS focus on efficiency and use the approach which assists you and your companies working practices.

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