User Defined Results in ANSYS Workbench — The Way to Make Your Simulation Results More Readable

点击此处查看 ✿水哥原创ANSYS视频教程清单 ✿

水哥专属答疑服务已开通，点此此处查看详情

In ANSYS Workbench post-processing, you can view many types of results. However, there are still some results that cannot be displayed through the default interface compared to APDL. Workbench provides the User Defined Results option to supplement these results.

To use this option, right-click on the Solution option and insert the User Defined Results. The user then inputs an expression to define the type of result to be viewed, as shown in the screenshot below.

The input expression is flexible, allowing for basic result operations such as addition, subtraction, and special result outputs. However, before using this feature, users need to understand the basic identifiers for expressions, such as UX for displacement in the X-direction.

So how can users view these basic identifiers? The answer is through the Worksheet option. In the Solution module, right-click and select Worksheet, which can also be found in the top menu bar.

The Worksheet is very useful for understanding the basic information of the overall structure, such as common element and material information. The first row lists all the outputtable result types, and if we need to use expressions, we mainly focus on the Expression column at the end. The Type and Data Type Component in the front of each row specify the basic information of the result, such as whether it is an element result or a node result, and which direction the result is in. In fact, this is a specific extension of the command flow PLNSOL and PLESOL, which can be compared by referring to their respective help documentation.

In addition to the basic PLNSOL and PLESOL options mentioned above, there are also some results that are output by default but not shown in the Worksheet. Users can refer to the help documentation for more information, and here are some screenshots.

With a basic understanding of the above expressions, it’s easy to combine results as desired. The expressions support the following types of operations (functions and geometric operators that are supported in APDL are also supported here):

1. Geometric operators: ‘+’, ‘-‘, ‘*’, ‘/’, ‘^’, ‘**’
2. Function operations: sqrt(), max(), min(), abs(), log10(), dot(), cross(), sin, cos, tan, etc.
3. Increase or decrease constants
4. User-defined expression operations

Next, let’s demonstrate some of these functions.

Demo 1: When viewing displacement results, in addition to the displacement in each direction, there is also a total displacement, which is the square root of the sum of the squares of the displacement in each direction. Let’s use a custom expression to verify this.

First, draw a cloud diagram of the total displacement as shown below:

Insert the user-defined result and enter the following expression:

(UX^2+UY^2+UZ^2)^0.5, and label the result as My_Results. As you can see, the two results are consistent.

Demo 2: Double the My_Results and then subtract 1.5 from all results, and label it as His_Results. The expression is as follows:

My_Results*2-1.5

Result verification:

The maximum value is 3.2329*2-1.5=4.9657, which is correct.

Demo 3: Take the minimum value of My_Results and His_Results.

The expression is as follows:

min(My_Results, His_Results)

As shown in the cloud diagram, the maximum value is 3.2329, and the minimum value is -1.5, which is as expected.

Good Luck!

欢迎搜索关注本站微信公众号：ANSYS结构院

欢迎给网站捐助，您的捐助是我坚持下去的动力！