+47 67 57 21 00
User Defined Result in ANSYS Workbench 2.0
ANSYS Tutorial:
How to extract desired results which are not directly accessible in Workbench but available for the element type we use, such as SMISC and NMISC outputs? In old days we had to do so by setting command snippet. But now with User Defined Result in Workbench 2.0 we can recreate easily all available results just under Solution. The article shows how.
TUTORIAL: Utilize User Defined Result in Workbench 2.0
We use a very simple structure to demonstrate the process. It is a square surface body with one edge fixed and uniformly distributed pressure on the surface:
By default ANSYS will mesh it with SHELL181. Here we need to simulate layered shell. So SHELL91 is the chosen element type. First insert a command snippet with following commands to 1) force ANSYS to mesh the surface body with SHELL91; 2) define 4 layers:
The default SHELL181 is 4-node linear element while SHELL91 is 8-node quadratic element. Do not forget to set Element Midside Nodes: Kept.
Again by default, Workbench will not write down all solution data. So we have to set one more command snippet to let Workbench to do so:
outres,all,all
After setting boundary conditions and load, we can define which result we need. User Define Result can be pre-defined in the same way as others:
We have to define Expression.
Expression? Wait a minute, what is it? OK, if we are experienced, we could fill it direct. But now we have totally no idea. So just delete the item with question mark and solve the model. When it is finished, first click Solution in the project tree and then choose Worksheet under the graphics windows. We will see a list of User Defined Result Expressions:
Don’t ask me why the Worksheet becomes activated only after solution is done. I don’t know. Anyway, I know now how expression looks like. We can extract User Defined Result by either filling expression such as UX, SX in the yellow field or right-clicking on the desired result and choose “Create User Defined Result”:
The list gives basic expressions. We can also combine them by using mathematical operators to further define the expression, such as UX+UY+UZ, sqrt(seqv), etc.
If we scroll down to the end of the list, we will find no SMISC and NMISC items. They can only be accessed by typing in the keyword directly. We have to check corresponding element description in the Element Reference to make sure exact expression. Back to our example, we will check interlaminar shear stress vector sum between layers. It is easy to find NMISC9 is for shear stress vector sum between layer 1 and layer 2. We define it as
Note, we give it an identifier “ilsum1”. An identifier is a user defined unique name which can be referred in the further usage. Furthermore, we rename the User Defined Result to ILSUM1. In the same way we can define shear stress vector sum between layers 2/3 and layers 3/4. Now we calculate maximum shear stress vector sum of all three interlaminations by a MAX function:
Expression in here makes use of the identifiers we defined earlier. After Evaluate All Results, we can get what we are looking for:
Do you want to learn more?
EDR provides a training course that covers basic Workbench operations, as well as other interesting topics.
Or contact our ANSYS Support to ask for hints!