For me and SW2016, SolidWorks inserts the variable name "$LIBRARY:MATERIAL@Part1" to specify a material in the design table and supplies values in the format "SOLIDWORKS Materials:ABS PC".
To get started, you can create two or more configurations, right-click on the material in the feature tree, and select "Configure Material". If you use at least a couple different materials for different configurations, next time you edit your design table SolidWorks will offer to create a "$LIBRARY:MATERIAL@Part1" column.
This worked out perfectly. When I went through the configuration publisher after what you informed me of I changed the parent name under visibility to the Thermowell length I created. Now when I open an assembly and select a part, I now have options to select a material to narrow down to the part number I am looking for. I appreciate the time you took to help my company and I with our dilemma.
Are all 3 parts of the probe the same material (stainless steel or brass)? If yes, then Dwight's answer is all you need.
But if the materials do vary, then make it a multi-body part (by unchecking "merge result" when doing each feature).
Now open up the Solid Bodies folder and right-click on each body. You can now click on Material and set it for each configuration.
When you edit the design table you will see a column like this for each body: "$LIBRARY:MATERIAL@Boss-Extrude1@Multi-Material Part"
And the $PRP@Weight will be the sum of all body/material combinations.