Creating a Reusable Parametric Component

June 11, 2020


Blog, NX CAM


Creating a Reusable Parametric Component

The reuse library has various uses such as housing common parts used within assemblies (i.e. hardware, clamps, pins, etc), features that are used routinely in your designs and / or have parameters preassigned to them, such as a feature color, or sketches that commonly used. Today, we will investigate the step required to create parametric components as well as adding them to a custom created Reuse Library.

Create Library Location: 

To keep your reusable parts organized in an efficient manner, Siemens provides the ability to create and manage the Reuse Library via the Reuse Library Management tool. This can be accessed via Menu →  Tools →  Reuse Library →  Reuse Library Management…

Here we can create a folder or folders to store our various part files. In the example I have created folder Swoosh_Reuse which is pointing to directory C:\02_customers\Swoosh\Swoosh_Reuse.

Create Parametric Part: 

The next step of this process is to create your part with parameters you would like to enter when you load the component from the Reuse Library.  In this example I am just creating a simple block with a chamfer on it. I have created 4 named expressions, length, width, height, and chamfer. These will be the four value to enter when using the component from the Reuse Library.

Next, I will link these expressions to part attributes. To do this right click on the part name in the Assembly Navigator → Properties. You will now create part attributes and link the expression to them by selecting Data Type – Expression Formula.

Save the part file to the folder we previously created for our own Reuse Library. In this case the location is C:\02_customers\Swoosh\Swoosh_Reuse.

Add Parametric Part to the Reuse Library: 

We will now navigate to our part file in our library. Chose the Reuse Library pallet on the Resource Navigator → Swoosh_Reuse. It may be necessary to refresh the contents of this folder, right click on Swoosh_Reuse → Refresh. Now we will create our .KRX file, this contains the attributes we need to populate for the instance of the component you will use.


We are also in need of a spreadsheet containing the default values we would like to use. Click the “Select a file” icon for the spreadsheet field, in the Swoosh_reuse folder create a new excel spreadsheet and name it the same as your part file. I enter the default values I desire; however, you can enter multiple values for each parameter if you’d like the ability to select from a pull-down list.

You will notice upon saving and closing the excel file, the “Primary Parameters” field is now populated. Press “OK”.

Open a new assembly part file to test your reusable component. From your Reuse Library, add your component to your new assembly file. The “Add Reusable Component” dialogue will launch and enable you to enter values as needed for the new instance of your component. Additionally, you can edit the values by right clicking on the component and selecting “Edit Reusable Component”.



Post by John Vincent

John's passion for understanding NX CAM has led him to become one of the most well-respected experts in the industry. His vast knowledge in post processing, mill manufacturing, and CNC programming is invaluable to manufacturing engineers and has earned him high praise from trainees looking to craft their knowledge. Did we mention he has his own show? (Tooling Time Season 1, Ep 1, Ep 2, Ep 3)

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