[ArslanOZCAN]

Hi guys.

I need to make transient cfd analysis of a vertical axis wind turbine in 2-D with sliding mesh method. I prepared a mesh and i think it is not the problem.

I prepared 2 different meshes. 1-Rectangular area with a hole in it. 2-Circular area containing airfoils. I opened these 2 meshes in FLUENT with append case file command. I will set rotational speed to the circular mesh. Now here are the questions;

-In mesh interfaces, should i use periodic or coupled?
-When i define mesh interfaces it sets 2 new wall boundary conditions.What are they and should they remain as wall?
-When i start solving it says turbulence viscosity is over than 1e05 in ... cells. And the number off cells increasing. What can be the problem.

Waiting for your commands...

[red_lemon]

-periodic I think but difficult to say without seeing grid
-walls need to become sliding interface so change to interface type and setup using define>mesh interface. Coupled wall will be thin non conformal wall
-check the grid is scaled correctly

[ArslanOZCAN]

I attached the picturese of my grid.
When i change these 2 walls to interface, it doesn't let me to add them in mesh interfaces. It says "CemberDis(name of the circle) is allready in another interface". When i just change them into interface and initiliaze the case it says "there are unassigned interface zones".

I checked and my grid is scaled correctly.

Waiting for your answer, and thank you...

[fivos]

Set the interface (from define -> grid interfaces) defining the two interface sides from the two meshes. In your case there is no need to select coupled or periodic so leave them un - ticked.

After setting the interface two new boundaries will be created, which are, by default, walls, as you have noticed. They are created because of the way fluent treats interfaces :
- It finds the intersection of the two adjacent interface boundaries
- The intersection is transformed to something like an "interior" boundary, to let information pass through
- The rest is transformed in wall. You can change this if you want by changing the newly created boundary to whatever you like.

Since in your case interfaces completely overlap (and you should make sure the interfaces do so), they will be transformed to the "interior" boundary and no wall will be created. You can simply omit the new boundaries, just as I said before, make sure that interfaces "touch" each other. Also try previewing the mesh motion to see if everything is all right.
Try running a few timesteps. Check if fluid flows through the sliding mesh by checking velocity, pressure contours etc in the sliding mesh.

For the turbulence viscosity, maybe you have to try lower relax factors, or smaller time step. It might vanish later on as simulation proceeds. How many cells have this problem (as a percentage of the total cells)? Where are these cells (plot turbulent viscosity from contours and see where they are)? What turbulence model do you use (initial conditions?, boundary conditions ?)?

Another comment on your mesh : I have seen from the first picture that your mesh at the stationary domain gets bigger near the interface. Why you didn' t use the smaller resolution used in the rest domain ?