CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > CFX

can I do this in CFX

Register Blogs Members List Search Today's Posts Mark Forums Read

Reply
 
LinkBack Thread Tools Display Modes
Old   August 15, 2010, 13:59
Default can I do this in CFX
  #1
New Member
 
koubaa
Join Date: Aug 2010
Posts: 7
Rep Power: 6
mohakou is on a distinguished road
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 is offline   Reply With Quote

Old   August 15, 2010, 16:09
Default
  #2
New Member
 
koubaa
Join Date: Aug 2010
Posts: 7
Rep Power: 6
mohakou is on a distinguished road
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 is offline   Reply With Quote

Old   August 16, 2010, 04:55
Default
  #3
New Member
 
koubaa
Join Date: Aug 2010
Posts: 7
Rep Power: 6
mohakou is on a distinguished road
Does anyone know if this is possible? If not I'm going to have to make an in-house code that does this =((((((
mohakou is offline   Reply With Quote

Old   August 18, 2010, 12:56
Default
  #4
New Member
 
koubaa
Join Date: Aug 2010
Posts: 7
Rep Power: 6
mohakou is on a distinguished road
nobody knows how to output a user defined variable at each iteration?
mohakou is offline   Reply With Quote

Old   August 18, 2010, 15:28
Default Mfx
  #5
New Member
 
Dr. Richard R. Lange
Join Date: Jun 2010
Location: Pittsburgh
Posts: 5
Rep Power: 7
DukeLeto is on a distinguished road
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.
DukeLeto is offline   Reply With Quote

Old   August 18, 2010, 15:35
Default
  #6
New Member
 
koubaa
Join Date: Aug 2010
Posts: 7
Rep Power: 6
mohakou is on a distinguished road
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 . 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 is offline   Reply With Quote

Old   August 18, 2010, 15:36
Default
  #7
New Member
 
koubaa
Join Date: Aug 2010
Posts: 7
Rep Power: 6
mohakou is on a distinguished road
Btw, coincidentally I am in Pittsburgh too lol, at UPitt
mohakou is offline   Reply With Quote

Old   August 18, 2010, 18:27
Default
  #8
New Member
 
koubaa
Join Date: Aug 2010
Posts: 7
Rep Power: 6
mohakou is on a distinguished road
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/DOMAINefault Domain/BOUNDARYefault 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, ...".)
mohakou is offline   Reply With Quote

Old   August 19, 2010, 08:40
Default Mfx
  #9
New Member
 
Dr. Richard R. Lange
Join Date: Jun 2010
Location: Pittsburgh
Posts: 5
Rep Power: 7
DukeLeto is on a distinguished road
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).
DukeLeto is offline   Reply With Quote

Old   August 25, 2010, 14:01
Default
  #10
Senior Member
 
Join Date: Apr 2009
Posts: 516
Rep Power: 12
stumpy is on a distinguished road
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
stumpy is offline   Reply With Quote

Old   September 17, 2010, 07:29
Default
  #11
New Member
 
Ali Bas
Join Date: Sep 2010
Location: İstanbul, Turkey
Posts: 15
Rep Power: 6
alialibas is on a distinguished road
Quote:
Originally Posted by mohakou View Post
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 is offline   Reply With Quote

Old   September 17, 2010, 07:32
Default
  #12
New Member
 
Ali Bas
Join Date: Sep 2010
Location: İstanbul, Turkey
Posts: 15
Rep Power: 6
alialibas is on a distinguished road
Quote:
Originally Posted by stumpy View Post
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???
alialibas is offline   Reply With Quote

Reply

Tags
cel, cfx, fsi, shear stress

Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Pros and Cons for CFX, CFdesign, COMSOL Val Main CFD Forum 3 June 10, 2011 02:20
CFX pressure in Simulations problem nasdak CFX 1 April 14, 2010 13:22
Importing solutions in CFX. Alphonso CFX 1 August 1, 2008 14:01
PhD using CFX Rui CFX 9 May 28, 2007 05:59
CFX 4.4 installation problem Pandu Sattvika CFX 1 December 1, 2001 05:07


All times are GMT -4. The time now is 16:56.