- All Categories
- How to create a volume location in CFD Post based on coordinates
Tagged: ansys-fluent, cfd-post, Volume location
June 6, 2022 at 8:33 amFAQParticipant
In order to define a volume location in CFD Post, one can use expression-based variables. There are two procedures:
1a) define an expression which has the value of 1 in the region to be defined as volume location, and value of 0 anywhere else.
For instance, expression which has a value of 1 in the region 0.25m < z < 0.75m and -0.025m < x < 0.025 can be defined as:
step((Z-0.25[m])/(1[m])) * step((0.75[m]-Z)/(1[m])) * step((X+0.025[m])/(1[m])) * step((0.025[m]-X)/(1[m]))
The function step(x) returns 1 when the x is positive, otherwise 0.
1b) define an expression based on the if function: if(Z<0.75 [m] && Z>0.25 [m] &&X<0.25 [m] && X>-0.25 [m],1,0)
2. define a new variable, select “Expression” as “Method” and choose the expression defined in step 1.
3. Insert -> Location -> Volume; select “Isovolume” as Method; Variable -> select the variable defined in step 2; Value = 1 Keywords: CFD Post, Volume, Iso-Volume, coordinates
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 EnSight: Overview of Postprocessing a Fluent Case in EnSight
- ANSYS Fluent: Simulation of a Rotating Propeller – Part 2
- 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
- ANSYS CFX: User Locations in Transient Simulations
- Comparison of Experimental and CFD data within ANSYS EnSight
- Add Annotation to Graphics Display within Fluent
- How can I calculate the average and difference between two data files using CFD-Post?
- How do I save a View?
© 2023 Copyright ANSYS, Inc. All rights reserved.