CFD Online Discussion Forums

CFD Online Discussion Forums (https://www.cfd-online.com/Forums/)
-   CFX (https://www.cfd-online.com/Forums/cfx/)
-   -   Interesting? TIME-AVERAGED VELOCITY STREAMLINE (https://www.cfd-online.com/Forums/cfx/201696-interesting-time-averaged-velocity-streamline.html)

heisenmech May 8, 2018 12:41

Interesting? TIME-AVERAGED VELOCITY STREAMLINE
 
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.

ghorrocks May 8, 2018 19:43

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.

heisenmech May 9, 2018 09:48

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?

Gert-Jan May 9, 2018 12:03

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?

nadernaderi June 13, 2018 16:39

Quote:

Originally Posted by heisenmech (Post 691647)
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.

heisenmech July 19, 2018 13:15

Quick Update
 
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


All times are GMT -4. The time now is 07:41.