How to define a Monitor Point in CFX-Pre based on its node number and then track a variable at this node.
June 5, 2023 at 7:05 amFAQParticipant
There’s a CCL only feature that allows you to attach a Monitor Point to a particular node. This is a beta feature that has been replaced with the Position Update Frequency option. More information about the Position Update Frequency option can be found in section 22.214.171.124.8.7. [Monitor Name]: Monitor Location Control, of the CFX-Pre User’s Guide in the ANSYS help documentation. The CCL for the old, beta method is: FLOW: OUTPUT CONTROL: MONITOR OBJECTS: MONITOR POINT: Monitor Point 1 Domain Name = Domain 1 Option = Vertex in Domain Vertex Number = 84634 Output Variables List = Total Mesh Displacement END END END END The Domain Name needs to match the name of the domain of interest. The variable of interest will often be Total Mesh Displacement, which will allow you to track the magnitude of the displacement of the selected node, but any variable can be entered. To find out a vertex (node) number at the point of interest, you can load the definition (.def) file into CFD-Post and then create a Point at the required XYZ location. After creating the Point, the nearest node number will be listed on the Geometry tab for the Point. If you don’t see this information then move the point slightly so that it lies within the mesh volume rather than on the mesh boundary.
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 can I create a Cell Register from a Cell Zone?
- Left-handed faces troubleshooting
- How to overcome the model information incompatible with incoming mesh error?
- ANSYS Fluent: Introduction to the GEKO Turbulence Model Part I
- Delete or Deactivate Zone in Fluent
- ANSYS System Coupling: Two Way Fluid Structure Interaction – Part 1
- How to create and execute a FLUENT journal file?
- Running Python Script from Workbench
- What are the requirements for an axisymmetric analysis?
- How to export plots automatically during a Fluent simulation using execute commands?