|
[Sponsors] |
Interesting? TIME-AVERAGED VELOCITY STREAMLINE |
|
LinkBack | Thread Tools | Search this Thread | Display Modes |
May 8, 2018, 12:41 |
Interesting? TIME-AVERAGED VELOCITY STREAMLINE
|
#1 |
Member
Oguzhan
Join Date: Aug 2017
Posts: 38
Rep Power: 9 |
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. |
|
May 8, 2018, 19:43 |
|
#2 |
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,852
Rep Power: 144 |
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. |
|
May 9, 2018, 09:48 |
|
#3 |
Member
Oguzhan
Join Date: Aug 2017
Posts: 38
Rep Power: 9 |
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?
|
|
May 9, 2018, 12:03 |
|
#4 |
Senior Member
Gert-Jan
Join Date: Oct 2012
Location: Europe
Posts: 1,910
Rep Power: 28 |
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 09:36. |
|
June 13, 2018, 16:39 |
|
#5 | |
New Member
nader
Join Date: Nov 2013
Posts: 9
Rep Power: 12 |
Quote:
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. |
||
July 19, 2018, 13:15 |
Quick Update
|
#6 |
Member
Oguzhan
Join Date: Aug 2017
Posts: 38
Rep Power: 9 |
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 |
|
Tags |
cfx & fluent, mean velocity, post procesing, streamlines, time-averaged value |
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
AMI speed performance | danny123 | OpenFOAM | 21 | October 24, 2020 05:13 |
Multiple floating objects | CKH | OpenFOAM Running, Solving & CFD | 14 | February 20, 2019 10:08 |
Time averaged velocity contour plots | tarkesdora | FLUENT | 0 | August 23, 2014 09:11 |
Micro Scale Pore, icoFoam | gooya_kabir | OpenFOAM Running, Solving & CFD | 2 | November 2, 2013 14:58 |
Upgraded from Karmic Koala 9.10 to Lucid Lynx10.04.3 | bookie56 | OpenFOAM Installation | 8 | August 13, 2011 05:03 |