- All Categories
- How do I separate out the pressure and shear force contribution to the force function.
June 6, 2022 at 8:33 amFAQParticipant
For the shear force (per unit area) there is variable called “Wall Shear”. Wall Shear is a vector variable with components Wall Shear X, Wall Shear Y and Wall Shear Z.
For the pressure force there is the scalar variable called Pressure. You can include the reference pressure by using the variable “Absolute Pressure” instead. You can convert the scalar pressure (force per unit area) into a vector by multiplying by the Normal vector variable.
So, for example
PressureForceX = Pressure * Normal X PressureForceY = Pressure * Normal Y PressureForceZ = Pressure * Normal Z
Sets up expressions that can be used to define scalar or vector variables. The normal vector typically points out of the domain and so will be pointing in the right direction (from fluid to wall).
There is a built-in Force vector that can be used to verify the accuracy of the pressure force vector or can be used as an alternative way to define the pressure vector using the following expressions
PressureForceX = Force X / Area – Wall Shear X PressureForceY = Force Y / Area – Wall Shear Y PressureForceZ = Force Z / Area – Wall Shear Z
This ensures the two forces (pressure and shear) sum exactly to the total force whereas the more direct expression for the pressure force only sums to the total to within the discretisation accuracy of the mesh. The force on any given boundary is then given by the area integral of the required force,
eg: WallForceX = areaInt(Pressure Force X)
A CFD-Post session file is attached which creates the expressions and variables needed. It creates a vector variable called “Pressure Force”. It also creates separate scalar variables for each component since it was discovered at version 2019R1 that posts reports that the components of a vector variable are undefined even though it correctly plots the vector.
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.
- ANSYS EnSight: Overview of Postprocessing a Fluent Case in EnSight
- How to create an Isovolume based on criteria from multiple variables
- How to get information about mesh cell count and cell types in Fluent?
- How to create a volume location in CFD Post based on coordinates
- How do I get experimental data into CFD-Post?
- How do I save a View?
- Can not create polyline with boundary intersection option. Warning: Cannot create a polyline. Outlet is not a boundary.
- How can I calculate the average and difference between two data files using CFD-Post?
- View External Airflow Around a Chevrolet Traverse SUS Using ANSYS EnSight
- How to create user defined volume in CFD Post?