Today’s blogpost for Simcenter 3D will be about how to obtain custom results from simulation files by using Result Probes. They enable the user to define new results based on the output from the solution. Here’s how:
Create the probe
Having defined a Solution you will have the option to create a Result Probe under Pre/Post→Results (tab)→Manipulation (group)→Result Probe, either before, or after solving the solution. All probes related to a specific Solution will be found under the Solution→Result Probes node in the Simulation Navigator.
First when you create a new probe you are asked for a name which must be unique within the same .sim file and if you would copy a Result Probe between solutions then suffixes will be added.
Define the Formula
After naming the probe, a formula input prompt comes with the option of defining new Result Variables. Right next to the input field of the formula there is an option of creating a Result Variable via the Create Result Variable button. Otherwise, they can be created via:
Pre/Post → Results (tab) → Manipulation (group) → Result Variables.
The Result Variables are non-solution specific entities specifying results to be used in the Result Probe. Meaning that one Result Variable can be used between different Result Probes in several different solutions. See an example below of a Result Variable extracting the von Mises stress on an elemental basis:
To define the Result Variable a unique name is required. For the data to be extracted we need to go through the following steps:
- Depending on the loaded solution’s results you will be able to filter between results applicable to that solution using the Result Filter and then select the Result Type.
- Location specifies whether we want to grab results from elements, element-nodes or from nodal entities. (These locations are applicable for structural stress analysis, there are additional locations)
- With the Location decided, first the result Datatype and thereafter the Component of that Datatype is set.
- Since this variable is set for solid structural elements Plies and Beam Result groups are left to their defaults
- The Combine At dropdown menu will enables us to average the results across element or node values.
- Not having any complex results Complex Options is also left to its default.
- Result Options gives you the option to obtain results in a select coordinate system and, if you want, the absolute result values.
Besides Result Variables, expressions can be used in the formula and without making this entire post revolve around expressions, here is a list of some of the entities which can define an expression:
- Constants; e.g. 4.00
- Functions; coming in several sub-categories of mathematical, lookup functions, as well as some more niche utility functions:
- Mathematical: COS(arg) – returning the cosine of the argument
- Lookup: YIELD(arg) – returns the element material dependent yield stress at temperature “arg”.
- Utility: REMU(arg) – returns the value from the expression defined by “arg” and simultaneously drops the unit of that value.
- Variables; these are predefined by SC3D and you reach them via the “ug_var” utility function. To lookup the variables possible to use in an expression open the Simulation Navigator → right click Fields → select Named Variables (Note, that many of the predefined variables share name with auto-generated expressions)
- Mathematical operators
All in all, the formula governing the output of the Result Probe can be made up of a combination of expressions and Result Variables for example:
| Formula | Involved entities |
| DX(“P_1”)-DX(“P_2”) |
|
| AVG(DX(“P_1”),DX(“P_2”)) |
|
| YIELD(85)/sig_vM_elemental |
|
Define the Result to Use for Output
Having a formula defining how to treat the result input to the Result Probe, next we need to define from where in the Solution to extract the result. Firstly, this needs to be done both with respect to when in time, or when in the solution sequence results are output. This is done using the Load Case selection as well as the Iteration Category and Iteration Selection. Secondly, we need to choose from which part of the model we want the results to come from: This is specified in the Selection and Averaging group with the Selection Type dropdown menu. Using the Combine Across Entities you also have the option of making this probe into a scalar quantity by combining results.
Specifying the Output
Finally, it is time to specify how we want the Result Probe to be output. First by handling entities without any results and secondly to specify Result Type and Unit. Lastly the Output Type is specified, depending on the Result Probe, to one of the following:
- List
- Post View
- Field
- Export Field
- UNV Export
- Graph
A Couple of Example Probes
Below you can review the videos to see examples of Result Probes defined for a SOL101 Solution
Safety Factor Based on von Mises Stress
Maximum Principal Stress Across Load Cases
Hope you found this Simcenter 3D tool useful in postprocessing your simulations and if you have questions about using Result Probes in your simulations reach out to support@volupe.com and we will be happy to help.
Viktor Hultgren, M.Sc.
Contact: support@volupe.com
+46 704 21 06 61
