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

Freezing 2-D, 2-phase, transient fluent simulation result to 3-D

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

Reply
 
LinkBack Thread Tools Display Modes
Old   December 10, 2015, 01:11
Default Freezing 2-D, 2-phase, transient fluent simulation result to 3-D
  #1
New Member
 
Amol
Join Date: Apr 2015
Posts: 4
Rep Power: 3
amolavid is on a distinguished road
Hello All,

I am simulating a 2D, 2-phase transient model with Moving Reference Frame in ANSYS Fluent 16.0. I want to freeze the time averaged volume fraction of second phase obtained from 2D simulation into a 3D domain.
Can anyone help me how to do this in Fluent??

Any help is really appreciated.

Thanks & regards,

Amol A
amolavid is offline   Reply With Quote

Old   December 10, 2015, 23:48
Default
  #2
Senior Member
 
Lucky Tran
Join Date: Apr 2011
Location: Orlando, FL USA
Posts: 1,372
Rep Power: 20
LuckyTran will become famous soon enough
You should be able to write an "interpolate" file. And then read this file into your 3D case. I think Fluent uses 0th order interpolation (nearest) which hopefully gives what you need. I still think you should perform some iterations on the 3D domain to get rid of any inaccuracies from the mapping procedure.

Do you already know how to freeze the variables after? You disable some equations, or use the freeze feature.
LuckyTran is offline   Reply With Quote

Old   December 13, 2015, 23:32
Default
  #3
New Member
 
Amol
Join Date: Apr 2015
Posts: 4
Rep Power: 3
amolavid is on a distinguished road
Hi LuckyTran,

Thank you so much for the reply and sorry I could not revert back as I was out of town.

Actually what I understand from your suggestion is that once I run 2D simulation, I can write an interpolate file for volume fraction of second phase and then import this file into a 3D domain.

What I really want is, I want to time-average the volume fraction of second phase for various times (e.g time-average volume fraction profile from say 0-2 seconds, 2-4 sec, 4-6 sec....). SO I will be having a different time-averaged profile at different times. Then I want to use these different profiles at different times in 3D simulation.

I hope I could make myself clear in what I really want to do.

Waiting for your reply.

Thanks and regards,

Amol





Quote:
Originally Posted by amolavid View Post
Hello All,

I am simulating a 2D, 2-phase transient model with Moving Reference Frame in ANSYS Fluent 16.0. I want to freeze the time averaged volume fraction of second phase obtained from 2D simulation into a 3D domain.
Can anyone help me how to do this in Fluent??

Any help is really appreciated.

Thanks & regards,

Amol A
amolavid is offline   Reply With Quote

Old   December 14, 2015, 00:47
Default
  #4
Senior Member
 
Lucky Tran
Join Date: Apr 2011
Location: Orlando, FL USA
Posts: 1,372
Rep Power: 20
LuckyTran will become famous soon enough
I don't remember if Fluent normally calculates the time-averaged volume fraction or not (maybe you can tell me, I am referring to the unsteady statistics option). If yes then you would still write the interpolate file the same way.

The only trick barrier is that Fluent treats the time-averaged and instantaneous variables at different named variables. So you would need to patch the instantaneous field with the time-averaged values. When patching zones Fluent doesn't let you reference the time-averaged quantities so you have to do a short workaround. Define a custom field function and set it equal to the time-averaged volume fraction. Then patch the instantaneous volume fraction with your custom field function.

If Fluent doesn't give the time-averaged volume fraction, then you need to solve that problem first.

Instead of an interpolate file, you can also write a profile.
LuckyTran is offline   Reply With Quote

Old   December 15, 2015, 00:28
Default
  #5
New Member
 
Amol
Join Date: Apr 2015
Posts: 4
Rep Power: 3
amolavid is on a distinguished road
Hi LuckyTran,

Fluent writes RMS values of volume fraction when we activate the tab "data sampling for time statistics" under run activities.

I could write the profile file of these RMS volume fraction of second phase. It gives me RMS values for different x and y co-ordinates. I will have to edit this profile file and add a third co-ordinate z and then will have to check if it works in 3D domain. But as far as I know, profile file works for patching of a face instead of domain.

For interpolate option, I wrote .ip file from 2D simulation. However, when I tried to import in 3D, it shows the error of "interpolation file has wrong dimensions". I am not able to read and edit this .ip file so as to add the theird dimension.
amolavid is offline   Reply With Quote

Old   December 15, 2015, 00:53
Default
  #6
Senior Member
 
Lucky Tran
Join Date: Apr 2011
Location: Orlando, FL USA
Posts: 1,372
Rep Power: 20
LuckyTran will become famous soon enough
Quote:
Originally Posted by amolavid View Post
Hi LuckyTran,

Fluent writes RMS values of volume fraction when we activate the tab "data sampling for time statistics" under run activities.

I could write the profile file of these RMS volume fraction of second phase. It gives me RMS values for different x and y co-ordinates. I will have to edit this profile file and add a third co-ordinate z and then will have to check if it works in 3D domain. But as far as I know, profile file works for patching of a face instead of domain.

For interpolate option, I wrote .ip file from 2D simulation. However, when I tried to import in 3D, it shows the error of "interpolation file has wrong dimensions". I am not able to read and edit this .ip file so as to add the theird dimension.
If it has RMS then it also has the time-average. Make sure you are using the time-average if that's what you need. The RMS in Fluent is the root-mean-squared fluctuations.

The .ip file is a simple ascii text file. You can open and edit it with any text editor (but your file might require a lot of memory to open). The detailed formatting and structure of the file is available in the Fluent help.

One of the first few lines in the .ip file is a 2 or 3 for 2D or 3D. Change it to 3 to see if you can read it as-is without adding the z-coordinate data.

If you know how to do an fscanf or fprintf in any programming language then it shouldn't be too hard to edit the file yourself to add the z-coordinate since it's a plain text file. There are lots of other and easier ways as well. Such as defining a dummy field variable, exporting it, and then renaming this variable to become the z-coordinate. You're going to do 0th order interpolation anyway so the z-coordinate can be anything. But you have to understand the format of the .ip file for it to work.

I haven't done a 3D profile either, I've always used a .ip file. I feel like it should work, but wouldn't beat myself up if I find out that it doesn't.
LuckyTran is offline   Reply With Quote

Old   December 23, 2015, 04:59
Default
  #7
New Member
 
Amol
Join Date: Apr 2015
Posts: 4
Rep Power: 3
amolavid is on a distinguished road
Hi LuckyTran,

Sorry for the late reply.

I read about the structure of the .ip file and could write a code to convert a 2D file into 3D. However, I need to test it before use it.

Meanwhile, I also wrote a 2D profile file, edited it to add a third dimension and imported it in 3D case, but I could not get any profile in 3D case.

Next thing I am gonna try out is to make a 3D case file with small z co-ordinate and then write a profile and interpolate file and import it in my actual 3D case to patch the volume fraction. Lets see if it works this way.

Please post if you also have something to approach this problem.

Thanks & regards,
Amol
amolavid is offline   Reply With Quote

Old   May 25, 2016, 10:37
Default
  #8
Member
 
enass
Join Date: Feb 2015
Location: Alexandria-Egypt
Posts: 30
Rep Power: 3
enass massoud is on a distinguished road
Quote:
Originally Posted by amolavid View Post
Hello All,

I am simulating a 2D, 2-phase transient model with Moving Reference Frame in ANSYS Fluent 16.0. I want to freeze the time averaged volume fraction of second phase obtained from 2D simulation into a 3D domain.
Can anyone help me how to do this in Fluent??

Any help is really appreciated.

Thanks & regards,

Amol A
Could you please tell me how to assign moving reference fram to two phase slug flow?
enass massoud is offline   Reply With Quote

Reply

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
looking for a smart interface matlab fluent chary FLUENT 17 December 2, 2016 21:26
Animation of Fluent transient data saisanthoshm88 CFX 19 April 21, 2016 21:57
Using FLUENT transient data in CFD-Post GJC075 FLUENT 0 November 25, 2013 10:56
transient simulation result file (.trn) ? amine CFX 3 June 14, 2008 05:01
Simulation of Two Phase Fluid Flow Problem Using Fluent 5.0 Mohammad Al-Shannag Main CFD Forum 1 July 16, 1999 11:28


All times are GMT -4. The time now is 15:55.