How to Use The SOLIDWORKS Configuration Publisher

Posted in: Mechanical Design
January 28, 2016

The Configuration Publisher is a SOLIDWORKS tool that filters through configurations using defining properties. On insertion, instead of choosing a configuration’s name, the Configuration Publisher prompts the user to choose parameters that filter which configuration is needed. This is particularly useful for parts and assemblies with many configurations that are used frequently. Configuration names that are of part numbers or are not descriptive enough to accurately determine which one is needed can also benefit from setting up a Configuration Publisher.

The steps in making the Configuration Publisher are very straightforward. After creating all of the desired configurations, right click on the component/assembly name in the Configuration Manager and choose Configuration Publisher as seen below:

1Figure 1: Select the Configuration Publisher

If a design table has not already been created, SOLIDWORKS will produce a prompt asking if one is needing to be auto-created as seen in figure 2.

2Figure 2: Prompt for creating a design table

The configuration Publisher box will then come up showing the different properties (controls) that can be used to filter through the configurations. These can be dimensions, materials, suppression states, etc. You then drag these controls from the left into the middle to use, while the edit tab is selected. (The process is the same for the Property Tab Builder).

3Figure 3: Left side of the Configuration Publisher holds the controls to drag in the edit box

Selecting a control in the middle allows editing its properties on the right. Here the variable on the design table is shown as well as the opportunity to change how the user sees the attribute name. This is seen in the figure below.

4Figure 4: Change the attribute name on the right

After editing is completed, the SW Preview tab will allow the user to view how the Configuration Publisher will display when initiated. When satisfied with the results, make sure to Apply the changes.

5Figure 5: Apply the changes

Now after inserting this part/assembly, SOLIDWORKS will prompt the user to choose through the set parameters to determine which configuration to pull in. As the parameters are chosen, Solidworks will filter through the remaining parameters available.

An example of this is shown below. For a length of 3, there are 2 configurations available. (Both have a 1.25 width) One is with a 1.25 hole and the other is with no hole. For a length of 4, only the default configuration is available, with a 1.5 width.

6Figure 6: 2 configurations available for a length of 3

7Figure 7: The default configuration is available for a length of 4

As the parameters are chosen, the part updates in the graphics area so the user has a visual of which part is being selected before it is chosen. If the chosen configuration needs to be changed and the user would like to utilize the Configuration Publisher to choose it, the menu can be brought back up by finding the part/assembly in the FeatureManager Tree, right click on it, and then choose Configure Part/Assembly from the in-context toolbar as seen in the figure below.

8Figure 8: Configure Part/Assembly

The configuration can still be chosen directly, if desired. When the part/assembly is inserted, the configuration can be chosen from the dropdown bar instead of sorting by properties.

9Figure 9: Configuration Name instead of Parameters

10Figure 10: Parameters listed for configurations

January 28, 2016
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