- Free Courses
- Learning Tracks
- Ansys Learning Hub
- All Categories
- Fluids - Postprocessing
- How can I calculate the average and difference between two data files using CFD-Post?
Tagged: Ansys CFD-Post
June 6, 2022 at 8:33 amFAQParticipant
This solution is applicable to both Fluent and CFX files.
1. Load two files in CFD-Post 2. Go to Tools > Compare Case, then turn on Case Comparison Active and click Apply. In the Variables tab, you will now see a folder called Difference which contains all difference variables. Note that the differences are always calculated as Case 1 minus Case
2. (More on Case Comparison can be found in section 12.8 Case Comparison of the CFD-Post User’s Guide.)
3. The *.Difference variable will be used to calculate the average. To demonstrate this algebraically, Temp1 will be the temperature variable for Case 1 and Temp2 will be the temperature variable for Case 2. The *.Difference variables are always calculated as Case 1 minus Case 2. Therefore, Temperature.Difference = Temp1 – Temp2 Note that the average temperature can be written as either: TemperatureAverage = (Temp1 + Temp2)/2 or TemperatureAverage = ((Temp1 – Temp2) + 2*Temp2)/2 Therefore: TemperatureAverage = (Temperature.Difference + 2*Temp2)
4. Create an User Defined variable which will represent the average temperature. To do this, right click under the Variable tab, then select New. Set the variable Method = Expression and the Expression = (Temperature.Difference + 2*Temperature). It is important to note that this variable will only be valid when plotted on Case 2. If this variable is plotted on Case 1, the expression will be equal to (Temperature.Difference + 2*Temp1) = (3Temp1 – Temp2)/2, which is incorrect.
5. To use this average temperature variable in an expression, the case and locator must be specified, for example: areaAve(TemperatureAverage)@CASE:2.Locator
6. The *.Difference variables are only created when CFD-Post is open and will not be saved to the data files. For CFX users, the *.Difference variables can be written to the .res file. To do this, in the Solver Manager, go to Tools > Interpolate Results and turn on Calculate Differences. The *.Difference variables will be written to the Modified Results .res file. These *.Difference variables will be equal to Modified Results – Original Results.
Introducing Ansys Electronics Desktop on Ansys Cloud
The Watch & Learn video article provides an overview of cloud computing from Electronics Desktop and details the product licenses and subscriptions to ANSYS Cloud Service that are...
How to Create a Reflector for a Center High-Mounted Stop Lamp (CHMSL)
This video article demonstrates how to create a reflector for a center high-mounted stop lamp. Optical Part design in Ansys SPEOS enables the design and validation of multiple...
Introducing the GEKO Turbulence Model in Ansys Fluent
The GEKO (GEneralized K-Omega) turbulence model offers a flexible, robust, general-purpose approach to RANS turbulence modeling. Introducing 2 videos: Part 1 provides background information on the model and a...
Postprocessing on Ansys EnSight
This video demonstrates exporting data from Fluent in EnSight Case Gold format, and it reviews the basic postprocessing capabilities of EnSight.
- How to get information about mesh cell count and cell types in Fluent?
- ANSYS Fluent: Simulation of a Rotating Propeller – Part 2
- ANSYS EnSight: Overview of Postprocessing a Fluent Case in EnSight
- How can I read a number of Fluent transient data files into CFD-Post as a single case?
- How to create an Isovolume based on criteria from multiple variables
- Add Annotation to Graphics Display within Fluent
- Display Multiple Plots in the Same Scene using Overlays in Fluent
- ANSYS CFX: User Locations in Transient Simulations
- Comparison of Experimental and CFD data within ANSYS EnSight
- Creating a User Surface in ANSYS CFD Post-processing