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

Interesting? TIME-AVERAGED VELOCITY STREAMLINE

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

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   May 8, 2018, 11:41
Cool Interesting? TIME-AVERAGED VELOCITY STREAMLINE
  #1
Member
 
Oguzhan
Join Date: Aug 2017
Posts: 36
Rep Power: 5
heisenmech is on a distinguished road
Hi everyone,

When I import Fluent transient solution file to CFD POST, I can display contours of time averaged variables (say velocity) without any issue. But when I try to display surface streamlines, there is no time averaged velocity option. All it offers me is colouring the streamlines with mean velocity. So my question is how one can display surface streamlines of time averaged velocity using Ansys CFD post?

Thanks.
heisenmech is offline   Reply With Quote

Old   May 8, 2018, 18:43
Default
  #2
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 16,346
Rep Power: 126
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
If you are doing a RANS simulation then the variable fields are time averaged, as per the Reynolds Averaging process.

If you want to average the flow field across a transient simulation - CFD-Post has no built in way of doing this. If you are using CFX you need to use the transient statistics output option to generate this. If you are using Fluent I have no idea how to do this.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
ghorrocks is offline   Reply With Quote

Old   May 9, 2018, 08:48
Default
  #3
Member
 
Oguzhan
Join Date: Aug 2017
Posts: 36
Rep Power: 5
heisenmech is on a distinguished road
Thanks Glen for your answer. Yes, tis a RANS simulation run with FLUENT which has an option called data sampling, which basically computes and saves time averaged scalars (which is pretty much the same thing as what CFX does). When I import my results to CFD-Post, I can see time averaged velocity contour without any issue, but cant plot time averaged surface streamlines. Any other post processing tool recommendation for this purpose?
heisenmech is offline   Reply With Quote

Old   May 9, 2018, 11:03
Default
  #4
Senior Member
 
Gert-Jan
Join Date: Oct 2012
Location: Europe
Posts: 1,171
Rep Power: 17
Gert-Jan is on a distinguished road
Isn't this is fluent problem? In other words:
Can you see the time averaged surface streamlines in Fluent?
Don't you have to save them explicitly as a non-standard variable, such that it becomes available in Post?

Last edited by Gert-Jan; May 10, 2018 at 08:36.
Gert-Jan is offline   Reply With Quote

Old   June 13, 2018, 15:39
Default
  #5
New Member
 
nader
Join Date: Nov 2013
Posts: 9
Rep Power: 8
nadernaderi is on a distinguished road
Quote:
Originally Posted by heisenmech View Post
Hi everyone,

When I import Fluent transient solution file to CFD POST, I can display contours of time averaged variables (say velocity) without any issue. But when I try to display surface streamlines, there is no time averaged velocity option. All it offers me is colouring the streamlines with mean velocity. So my question is how one can display surface streamlines of time averaged velocity using Ansys CFD post?

Thanks.
There is no direct way to plot streamlines using time averaged velocity values in CFD Post. But a workaround can be as follows:
Create 3 custom field functions. Let’s say
cff1 = Mean U velocity
cff2 = Mean V velocity
cff3 = Mean W velocity
Now you can go to initialize and then use the patch functionality to patch the X, Y and Z velocities to cff1, cff2 and cff3 respectively. Once that is done, export the velocities in CFD-Post compatible format and then plot streamlines using the velocities.
nadernaderi is offline   Reply With Quote

Old   July 19, 2018, 12:15
Smile Quick Update
  #6
Member
 
Oguzhan
Join Date: Aug 2017
Posts: 36
Rep Power: 5
heisenmech is on a distinguished road
Hi again,

Just popped back here to my question to give a brief update. Ive tried all the possible ways that I can think of and that people here suggested. But none of them worked :/ (or I was doing sth wrong). The most straight forward solution is in Tecplot. BUT! If you save and import your data as Tecplot compatible, you wont be able to perform slicing in Tecplot, which is pretty stupid. So, when you launch the Tecplot go for the Fluent Data Loader and import data.Then, specify the plane that you want to see the streamlines on. Next, go click on the streamtraces and you'll be asked to select variables. For instance, select mean X, mean Y and mean Z velocities s(these mean values should be extracted from Fluent by enabling data sampling) for U, V and Z components. Enjoy your streamlines of time-averaged velocity!!

Best,
heisenmech
heisenmech is offline   Reply With Quote

Reply

Tags
cfx & fluent, mean velocity, post procesing, streamlines, time-averaged value

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
AMI speed performance danny123 OpenFOAM 20 April 10, 2020 05:51
Multiple floating objects CKH OpenFOAM Running, Solving & CFD 14 February 20, 2019 09:08
Time averaged velocity contour plots tarkesdora FLUENT 0 August 23, 2014 08:11
Micro Scale Pore, icoFoam gooya_kabir OpenFOAM Running, Solving & CFD 2 November 2, 2013 13:58
Upgraded from Karmic Koala 9.10 to Lucid Lynx10.04.3 bookie56 OpenFOAM Installation 8 August 13, 2011 04:03


All times are GMT -4. The time now is 06:25.