How do I create a domain interface when the two sides of the interface have the same mesh location, i.e. a conformal interface?
June 6, 2022 at 8:33 amFAQParticipant
If you want to add an interface between two domains and do not want to use the automatic interfaces (maybe because you only want a subset of the faces), you will want to add named selections for the two sides especially if there are a large number of faces. This is ok if the domains are obtained from different parts at the meshing stage, but if they are meshed within a single part the mesher will have a single location to represent both sides so the named selection will end up with faces from both sides of the interface. What is the easiest workaround?
1) Create the name selection on the interface, this will be loaded into CFX but will have faces from bodies on both sides of the interface (therefore double the number required).
2) Create an interface between the two domains and add 2 faces as place holders.
3) Expand the mesh section at the top of the tree and in the Other 2D regions section and locate the named selection. Open the name selection, in the regions list highlight all of the locations and type Ctrl-C to get ready to copy the regions names.
4) Go to the interface of interest, right click on it and select “Edit in Command Editor”. This wil bring up the CCL for the section.
5) In Interface Region List 1 =F***.*** delete the existing location and use Ctrl-V to paste in the copied location names (note that this will include both sides).
6) Repeat for Interface Region list 2, so now both sides have both sets of faces.
7) At the top of the window, change Filter Domain List 1 and 2 so instead of 1 being DomainA and 2 DomainB set both to be “DomainA, DomainB” (include all domains from both sides of the interface). This is needed to avoid problems caused by listing faces that are not permitted by the filter settings.
8) Click on Process. This will read in the new settings and set both sides of the faces to both sides (which will produce another error message).
9) Open the interface in the standard gui (double left click). Change the filters so that List 1 is Domain A and List 2 is Domain B. (This should automatically divide the faces between the two sides.) Click OK.
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.
- Solver message during DPM calculation: “number of stepsize underflows during particle integration step is x”. What does it mean and how to get rid of it?
- ANSYS Fluent: Efficient Modeling of Spray Breakup using VOF-to-DPM Transition
- ANSYS Fluent: Describing Cavitation in a Centrifugal Pump
- Simulation of Exhaust Gas Recirculation (EGR) Cooler with CFD
- Mixing Tank Modeling in ANSYS Fluent
- ANSYS Fluent: Lifeboat Launch – Overset & Dynamic Meshes with the Volume of Fluid Model
- Hydrodynamics and Wave Impact Analysis
- Optimizing Solid Distribution in Continuous Stirred-Tank Reactor
- ANSYS Fluent: Simulating Multiphase Mixing within a Sparging Tank – Part 1
- ANSYS Fluent: Simulating Multiphase Mixing within a Sparging Tank – Part 2