can I do this in CFX
Hi,
This is a two-way FSI problem. I am working on a model of a theoretical wall material who's temperature depends on the wall shear stress introduced by the fluid. I tried using expressions to make an 'Additional Variable' which depended on Shear stress but had units of temperature. In the boundary details panel I tried sending the 'Additional Variable' as the CFX variable into the ANSYS 'TEMP' variable. There is absolutely no thermal boundary conditions or conductivity, etc. in the fluid model as this is not important for this test. The problem I ran into was that it does not allow me to send my variable in the 'Additional Coupling Sent Data' section. Anything I'm missing? Thanks |
Main problems I've had with this approach is I don't know how to access the shear stress value at each iteration. Do I need to call it with a function? Once I am able to get it, and use expressions to get a variable that is a function of the wall shear, I can just edit the mfx input file so that the CFX label in the mflc command is the variable that I end up with, right?
|
Does anyone know if this is possible? If not I'm going to have to make an in-house code that does this =((((((
|
nobody knows how to output a user defined variable at each iteration?
|
Mfx
It is not clear that this is a two way FSI problem. How is the fluid region being affected by the wall material? Is it deforming significantly?
If the temperature is not important to the fluid, perhaps you could calculate your desired quantity and set the CFX temperature to this with an expression. The ANSYS side will consider this as an actual temperature, however. MFX is pretty narrow in focus. |
Thanks for the reply. I'm expecting the wall to deform significantly, so ideally it would have to be 2-way fsi. I think, if I'm not mistaken, the CFX temperature is only available if I have some kind of thermal analysis setup :mad:. But you're right, if the CFX temperature was calculated internally then I wouldn't have to do anything fancy with the MFX. I'll doublecheck if I can't find anything in the docs or if nobody here knows for sure
|
Btw, coincidentally I am in Pittsburgh too lol, at UPitt
|
Tried to put in temp under the 'additional coupling data sent' in the command editor (of the analysis). Apparently it just won't accept to send temp to ansys. This is the error message I got when I processed the command.
The parameter "CFX Variable" in "/FLOW:Flow Analysis 1/DOMAIN:Default Domain/BOUNDARY:Default Domain Default/COUPLING DATA TRANSFER:temp" holds the following disallowed value: "TEMP". (Allowed values are: "Total Force, Total Force Density, Total Force Density X, Total Force Density Y, ...".) |
Mfx
By all means, let CFX calculate the energy equation. It should simply reproduce the results of the expression that you have created (a version of "the all-important-trivial-case"). Certainly without the energy equation, it won't want to send temperature. Just make sure your fluid properties are not a function of temperature or pressure (e.g. no ideal gas).
|
Sending an AV to the ANSYS "TEMP" variable worked OK for me. Here's the bits of CCL:
LIBRARY: ADDITIONAL VARIABLE: Additional Variable 1 Option = Definition Tensor Type = SCALAR Units = [K] Variable Type = Unspecified END END FLOW: Flow Analysis 1 DOMAIN: Default Domain FLUID MODELS: ADDITIONAL VARIABLE: Additional Variable 1 Additional Variable Value = 2*Temperature Option = Algebraic Equation END END END END FLOW: Flow Analysis 1 DOMAIN: Default Domain BOUNDARY: Default Boundary Boundary Type = WALL BOUNDARY CONDITIONS: HEAT TRANSFER: Option = Adiabatic END MASS AND MOMENTUM: Option = No Slip Wall END MESH MOTION: ANSYS Interface = FSIN_1 Option = ANSYS MultiField Receive from ANSYS = Total Mesh Displacement Send to ANSYS = Total Force END WALL ROUGHNESS: Option = Smooth Wall END END COUPLING DATA TRANSFER: Coupling Data Transfer 1 ANSYS Interface = FSIN_1 ANSYS Variable = TEMP CFX Variable = Additional Variable 1 Coupling Data Transfer Type = Profile Preserving Option = ANSYS MultiField END END END END |
Quote:
You can transfer the heat by using Heat transfer option as a Multifield in CFX. But in your mechanical input file must be created to be able solve heat problem. i think it must be prepared under multiphysics licence, i think... you dont need to add an additional variable.. |
Quote:
|
All times are GMT -4. The time now is 02:56. |