In fluent create iso-surface for wake. Goto menu display>graphics and animation > contours. select the parameter/property your want then select the wake just created for surface. adjust manually the range of values. there are your contours.

Hve you tried inserting streamlines or vectors?

ya i did stream lines and vectors. but I cant get the wake structure

Try q-criterian and lambda criterian

Can u pls explain me in detail in fluent

Sorry. I use cfd-post for post-processing. This option is available in cfd-post and not in fluent.

You can compute Q-values in your domain. I have copied the text from another source to facilitate you in Fluent usage. You are welcome to ask if you need further guidance on Q-criterion.

"Fortunately, you don't have to use UDF. Here's a simpler way of visualizing the iso-contours of the second-invariant. You can use the custom field function capability in FLUENT. First you define the second-invariant of deformation tensor with Q = 0.5(W*W - S*S) where W is the vorticity magnitude (you can find it under the "Velocity" menu) and S is the mean rate-of-strain (you can find it under "Derivatives" menu). Once you defined Q, you can generate iso-surfaces of Q for several positive values."

Hope it helps

Try iso-surface of Lamda2 or Q-criterion

Start Workbench, drag Fluent icon to the Workbench workspace, set up and solve your problem, after your solution has converged, go to Workbench and right click on Setup tab from Fluent > Transfer Data To New > Results, access Results (CFD Post) from Workbench, click Location > Vortex Core Region, choose from drop-down menu what you are interested in.

Thanks all for ur reply

As there are number of post processor available but from them i used surfer , cfd -post,para-view & tech plot out of these i feel tech plot is much user friendly and its easy to deal with it but as availability of cfd-post with ansys so mostly people use that for post processing but that have some limitation.

I hope your problem is solve .

In fluent create iso-surface for wake. Goto menu display>graphics and animation > contours. select the parameter/property your want then select the wake just created for surface. adjust manually the range of values. there are your contours.

Here's the best way:

Step 1: When you setup the simulation in CFX Pre; go to >>Output Control >> Extra Output Variables List. Select: Vorticity, Vorticity X, Vorticity Y and Vorticity Z. This gives the vorticity about each principle axis, and the total magnitude of vorticity.

Step 2: When you do your post processing you should use coordinate transforms to determine the vorticity in the cylindrical coordinate system of the rotor. Assuming you use z for the axial direction: (x,y,z)->(r,\theta,z). Create "Expressions" for vorticity r, and vorticiy theta to define the transforms. Then go to the "Variables" Tab, right click and add "new" variables: Vorticity R, Vorticity Theta, using the method "expression". 

Now you can plot the vorticity about R and about theta. This is useful because the bound vorticity of the blade is about the radial direction, while the trailed vortices in the wake, (e.g. tip-vortices) are mainly about the azimuthal direction (Theta). The vorticity about z (assuming z is your axial direction) will correspond to the swirl in the wake (strongest at the wake centre).

If you want to do quantitative analysis on the trailed vortices, you could do more sophisticated coordinate transforms to get the vorticity about streamlines trailed from the blades. 

Vorticity can be  plotted using fluent post process or export vorticity directly to tecplot. Menu or command structure depends on the version that is being used. Refer manual  related to plotting contours/ reports or exporting the data.

You can try isosorface of q-criterion or lambda2 to visualise the development of vorticity

Dear colleagues,

i have an another  question about CFD POST 

When we start CFD POST we receive this message:

" Note that for files other than CFX-Solver Results, global ranges are calculated for the used variables and the currently loaded timestep only. As more timesteps are loaded, global variable ranges are adjusted dynamically. Tip: To avoid dynamic range updates, you can use local variable ranges, or turn on pre-calculation of global ranges for all timesteps and all variables in : Edit>Options>CFD-Post>Files"

it means that for files other than CFX ( FLUENT for example ) we have to change dynamically the range of  variables by going to Edit>Options>CFD-Post>Files and we check " Pre-calculate global variables ranges " .

in my unsteady simulation I have different time steps results and I want to show them , but when I follow the steps that I cited above in order to change dynamically the variables range for each time step it doesn't work and i got the same results for all the time steps !!! 

Please if someone has encountered the same problem and has found a solution please help me.

Thank you .

Hi there,

By definition the vorticity is a pseudovector field that describes the local spinningmotion of a continuum near some point (the tendency of something to rotate. In FLUENT is given by : dY-Velocity/dx minus dX-Velocity/dy.

To plot contours for this function using FLUENT go to the "Define" menu, pick "Custom Field Function". Then in the "Field Functions" drop-down box, pick "Derivatives", select "dY-Velocity/dx" from the second drop-down box, click "Select", then the "-" button, then select "dX-Velocity/dy " and click "Select".

Now choose a name for your new variable (e.g. "Vorticity-signed"), then click "Define".

When you go to plot contours, choose "Custom Field Functions", and your new variable will be available. Note that most of the vorticity will be in the boundary layer, so you will probably have to take it off "Auto Range" and pick some lower values to see anything at all in the wake. Positive values represent rotation in one direction, negative values in the other.

Hope this helps,

Sohaib