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

CFX - specified domain intialization

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

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   September 28, 2020, 05:30
Default CFX - specified domain intialization
  #1
New Member
 
qntldoql
Join Date: Sep 2020
Posts: 15
Rep Power: 4
qntldoql is on a distinguished road
Hi,

I have read up other post related to this problem, but couldn't find an answer (or the answer didn't work for my scenario).
My problem is, I have a steady state results that I want to use it as an initialization file for the transient simulation.
For the transient case, I have introduced an another domain that surrounds the domain of the SS file. (I'm trying to observe the interaction between the two domains)
Therefore, I want to use the SS result file to initialize ONLY the same domain in the new simulation.

From the other posts, apparently I should only initialize the domains that I do not want to be initialized by the res file. I have done that. But when I run the simulation, res file successfully initializes the same domain, but also interpolates onto the domain that I have already specifically initialized in pre.
I was wondering if anyone possible has a solution to this problem.



================================================== ====================
Interpolating Onto Domain "Default Domain"
================================================== ====================

Total Number of Nodes in the Target Domain = 943936
Bounding Box Volume of the Target Mesh = 3.73042E-01


Checking all source domains from the source file:
Target mesh is the same as domain "Default Domain".

Start direct copying of variables from domain "Default Domain".
================================================== ====================
Interpolating Onto Domain "X"
================================================== ====================

Total Number of Nodes in the Target Domain = 602518
Bounding Box Volume of the Target Mesh = 3.04070E+00


Checking all source domains from the source file:
Target mesh is different from domain "Default Domain".

Searching for Candidate Source Domains:
Domain "Default Domain"
Number of Mapped Nodes = 2923 ( 0.5%)
Bounding Box Overlap Volume = 3.73042E-01 ( 12.3%)
Setting Up Unmapped Nodes:
Number of Unmapped Nodes = 599595 ( 99.5%)

Start interpolation of variables:
Source Domain Name Mapped Nodes
Default Domain 2923 ( 0.5%)



Default domain X above is the one I do NOT want to be initialized by the res file.

here's the pre of the domain X:
INITIALISATION:
Option = Automatic
INITIAL CONDITIONS:
Velocity Type = Cartesian
CARTESIAN VELOCITY COMPONENTS:
Option = Automatic with Value
U = 0 [m s^-1]
V = 0 [m s^-1]
W = 0 [m s^-1]
END
STATIC PRESSURE:
Option = Automatic with Value
Relative Pressure = 1 [atm]
END
TEMPERATURE:
Option = Automatic with Value
Temperature = 293 [K]
END
TURBULENCE INITIAL CONDITIONS:
Option = Low Intensity and Eddy Viscosity Ratio
END
END

I also read that I should set the option as 'Value'. But only available options are 'Automatic' or 'Automatic with value' for me. Tried to see if I can add it as 'Value' in the commander editor but I could not.
qntldoql is offline   Reply With Quote

Old   September 28, 2020, 08:59
Default
  #2
Senior Member
 
Join Date: Jun 2009
Posts: 1,641
Rep Power: 29
Opaque will become famous soon enough
Setup the initialization using Automatic with Value,

Use Edit in Command Editor, delete the "Automatic with" from the option, and process. Then, close.

You should get a physics error in the window about invalid Option = Value, only valid options are....

Ignore the error, and proceed to write the definition file and start the simulation. It should work.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
Opaque is offline   Reply With Quote

Old   September 28, 2020, 09:22
Default
  #3
New Member
 
qntldoql
Join Date: Sep 2020
Posts: 15
Rep Power: 4
qntldoql is on a distinguished road
I tried it using your suggestion of replacing all of the "automatic with value" with "Value" in the command editor.

INITIALISATION:
Option = Automatic
INITIAL CONDITIONS:
Velocity Type = Cartesian
CARTESIAN VELOCITY COMPONENTS:
Option = Value
U = 0 [m s^-1]
V = 0 [m s^-1]
W = 0 [m s^-1]
END
STATIC PRESSURE:
Option = Value
Relative Pressure = 1 [atm]
END
TEMPERATURE:
Option = Value
Temperature = 293 [K]
END
TURBULENCE INITIAL CONDITIONS:
Option = Low Intensity and Eddy Viscosity Ratio
END
END

It does show following "error" lines in the window:
Parameter "Option" in ..... has the value "Value". This does not match any of the allowed values ....
and
The parameter "relative pressure, T ..." is present in object '.." but it is not physically valid.

I ignored these messages and worked with the def file as suggested, but it still interpolates the res file values onto the unwanted domain. (identical output as the first post). I also tried to initialize the domain that I do want to initialize by not initializing and initializing with automatic with value, but it still interpolates to both domains. How should I proceed?
qntldoql is offline   Reply With Quote

Old   September 28, 2020, 09:41
Default
  #4
Senior Member
 
Join Date: Jun 2009
Posts: 1,641
Rep Power: 29
Opaque will become famous soon enough
Probably does that, but it should still use your data for Value.

For verification, you should write a backup file at start of the run to verify which initial conditions were applied.

Check for expert parameter about writing the backup file at the start of the run, or at iteration 0.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
Opaque is offline   Reply With Quote

Old   September 28, 2020, 10:28
Default
  #5
New Member
 
qntldoql
Join Date: Sep 2020
Posts: 15
Rep Power: 4
qntldoql is on a distinguished road
You were right!
I proceeded with the run with the monitor point on a domain that I have initialized (not wanted to be interpolated from the res file). And it shows the input temperature (293k) for the first few runs!
Thank you very much!
qntldoql is offline   Reply With Quote

Reply

Thread Tools Search this Thread
Search this Thread:

Advanced Search
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 Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Can CFX model periodic heat transfer problem Ethan_Sparkle CFX 41 June 14, 2017 08:22
Periodic Pressure drop cfd_begin CFX 10 May 25, 2017 08:09
Out File does not show Imbalance in % Mmaragann CFX 5 January 20, 2017 11:20
ANSYS CFX Solver Domain Imbalance amodpanthee CFX 9 March 8, 2016 18:55
Error finding variable "THERMX" sunilpatil CFX 8 April 26, 2013 08:00


All times are GMT -4. The time now is 08:27.