Hi all,

I am simulating an oscillating cylinder and observing the vorticities. Does anyone know how to view the velocity in which the clock wise and anti clockwise vorticity direction gives you diff colour in the contour plot? This will make it easy to differentiate between positive and negative vorticity direction.

Sham

Hello,

Your question is not entirely clear to me. However, if you want to look at the direction in which the vortices are rotating (i.e. whether clockwise or counter-clockwise) why not plot the velocity vectors?

Hi Sham, I'm assuming your problem is 2D, where fluent only provides the vorticity magnitude. To get around this you can define a Custom Field Function (see sect 30.5.1 of the user guide) for the vorticity which is du/dy - dv/dx. John

John,

Could you pls explain a little bit more how can I use the Custom Field Function to define the vorticity direction and show it in diff colour? I am modelling a 2D cylinder in free stream.

Sham.

Hi Sham,

Go to the "Define" menu, pick "Custom Field Function". Then in the "Field Functions" drop-down box, pick "Derivatives", select "dX-Velocity/dy" from the second drop-down box, click "Select", then the "-" button, then select "dY-Velocity/dx" 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 that helps, John

John,

Thanks a lot. It works.

Sham.

[anil raj]

I have one doubt regarding the vorticity calculation in FLUENT. In a forum i found the vorticity calculation is by du/dy-dv/dx. But this is valid for structured mesh only according to theory and how can it be valid for unstructured grids. Is there any method (Algorithm) by which Fluent calculates the vorticity for unstructured grid?.

[rajann_786]

To, John Young
Thanks!!! It is helpful.

[adilio]

Thank You John
I lost my 3 weeks finding how to do this.. finally you made my day

[Mahram Khan]

Originally Posted by anil raj

I have one doubt regarding the vorticity calculation in FLUENT. In a forum i found the vorticity calculation is by du/dy-dv/dx. But this is valid for structured mesh only according to theory and how can it be valid for unstructured grids. Is there any method (Algorithm) by which Fluent calculates the vorticity for unstructured grid?.

How did you define vorticity for the unstructured mesh?

[LuckyTran]

Originally Posted by Mahram Khan

How did you define vorticity for the unstructured mesh?

The vorticity is defined mathematically the same way regardless of mesh. What differs is how you would actually go and calculate the gradient field. Fluent is an unstructured solver anyway, so it never matters. Whether your mesh is structured or not, Fluent treats it like an unstructured mesh.

[Mahram Khan]

Originally Posted by LuckyTran

The vorticity is defined mathematically the same way regardless of mesh. What differs is how you would actually go and calculate the gradient field. Fluent is an unstructured solver anyway, so it never matters. Whether your mesh is structured or not, Fluent treats it like an unstructured mesh.

I have defined the vorticity same way and there is one built-in function for vorticity magnitude, I have compared the results and it differs on a few nodes. Can you please explain why it differs on a few nodes. Thanks!

[LuckyTran]

Originally Posted by Mahram Khan

I have defined the vorticity same way and there is one built-in function for vorticity magnitude, I have compared the results and it differs on a few nodes. Can you please explain why it differs on a few nodes. Thanks!

on notes or on cells? On nodes, there's all sorts of wonky interpolation that happens.

[Mahram Khan]

Originally Posted by LuckyTran

on notes or on cells? On nodes, there's all sorts of wonky interpolation that happens.

Yes, it was on nodes, however, on cells it's same. Thanks!

[Mahram Khan]

Originally Posted by LuckyTran

on notes or on cells? On nodes, there's all sorts of wonky interpolation that happens.

Can I ask you one more thing? What model is the best for 2D unsteady simulations in order to verify Navier-stokes equations? Thanks!