CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   CFX (http://www.cfd-online.com/Forums/cfx/)
-   -   can I do this in CFX (http://www.cfd-online.com/Forums/cfx/79173-can-i-do-cfx.html)

mohakou August 15, 2010 13:59

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

mohakou August 15, 2010 16:09

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?

mohakou August 16, 2010 04:55

Does anyone know if this is possible? If not I'm going to have to make an in-house code that does this =((((((

mohakou August 18, 2010 12:56

nobody knows how to output a user defined variable at each iteration?

DukeLeto August 18, 2010 15:28

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.

mohakou August 18, 2010 15:35

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

mohakou August 18, 2010 15:36

Btw, coincidentally I am in Pittsburgh too lol, at UPitt

mohakou August 18, 2010 18:27

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, ...".)

DukeLeto August 19, 2010 08:40

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).

stumpy August 25, 2010 14:01

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

alialibas September 17, 2010 07:29

Quote:

Originally Posted by mohakou (Post 271548)
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

hi,
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..

alialibas September 17, 2010 07:32

Quote:

Originally Posted by stumpy (Post 272733)
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

I am confused with your ccl. i am not so good in this programe. but you prepare it as a adiabatic? but trying to transfer heat by an additional variable? is't is possible by using "Heat Transfer" option in CFX as a "Multifield" option???


All times are GMT -4. The time now is 02:49.