[ghorrocks]

As I have said previously, your difficulty in converging is a FAQ: http://www.cfd-online.com/Wiki/Ansys...gence_criteria

[miquiita]

I know it is a convergency problem, but I tried to take the physical time step and the convergency then looks like this picture that I stoped due to the unsteady curve of the plot. Then I changed to local timestep of 3 and the convergency went below the 1e-4 after about 194 iteration and the result look like the flow in the duct. I read all the convergency doc and help files and I cannot seem to get the problem why my physical time step of L/v (2.67) does not converge properly. And why I should not use the local time step.

There is a hole in the outlet of the flow as can see in one of the pics, I have no idea why, because I use the local time step?

[ghorrocks]

I do not know what is your inlet or outlet and I do not know what hole you are talking about.

In the FAQ you appear to have missed:
* You should not use local time stepping for the final run to convergence, you should switch back to physical time step - search the forum for the reason why not.
* You probably need a larger physical time step to assist convergence.
* You have already converged your results now to a low level of accuracy. But this may be acceptable for what you are trying to do - you will have to assess that.
* If the suggestions above do not help then you probably need to run this transient to get final convergence.

This is all described in the FAQ.

[miquiita]

I saw that step, but my physical time step is not working. Inlet is the one with the fluid is blue and outlet is where the lighter blue is.

Thanks, I am not sure what I will assess to make sure it is good enough for what I am suppose to get. I just wanted to see if the rotor geometry is good for a fan by plotting the pressure and flow velocity in a graph, to see the velocity for the fan and not a turbine.

I tried the physical time step, a too big one gives me an error.

Thanks, I am sorry for not understanding all of it.

[ghorrocks]

Another issue you need to consider - there is a lot of rotation in the flow upstream and downstream of the fan. Is this what you intend? Most fans are designed to minimise flow rotation as it is wasted energy.

[miquiita]

Hi,

I do not want to much rotation, if it is not comparable to reality, which it is not. But my main purpose of the simulation before putting the rotor in a room, is be sure of the geometry is valid of the rotor.

How would I minimise the rotation then? I know if I lower the velocity is might work. Or should I shorten the duct?

thanks

[ghorrocks]

Before you do any CFD you need to define what the inlet and outlet flow conditions are on the experiment you wish to model. This includes what swirl the inlet flow has. You then need to define boundary conditions which match the experimental conditions.

So do you know what conditions the flow you are trying to model was produced in?

[miquiita]

I got the assignment to model a flow in a duct of a fan, with inlet as normal velocity and outlet as 0 static pressure (which now in the model wants to be an opening).

This model is not based on experiment it is more based on as before checking the geometry of the fan blade. But I was trying to find a duct and a axial fan paper, to have as a base to compare results with but could not find a similar one that been published.

[ghorrocks]

What boundary conditions have you applied? Even better, please attach your CCL.

[miquiita]

OK here is the CCL. I treid so many different methods and now I refined the mesh in this one, I have inlet as normal speed. Outlet as a opening with entrainment. Then I got 1.5 m/s as the speed of inlet. I have the physical timestep as 4, due to my duct is 6 meters.

I run the model as steady state, but the flow never develops in the outlet and also the flow is really circular motion of inlet too. Was more hoping to get something like a steady flow inlet that then swirls the flow after the fan, more realistic to a fan.

[miquiita]

Here is the CCL file.

[ghorrocks]

Note that the comments in the CFX documentation about setting physical time step to a typical residence time is just a starting point. From there you adjust it depend on what you see - if it looks unstable you go smaller, if it is stable but converging slowly you make it larger.

Have you had a close look at the flow in the fan to see if the flow is operating as designed (ie attached flow) or if you are way off the design point (ie separations)?

[miquiita]

Hi I know that and I tried increasing the timestep, but the model stops running with an error code of overflow, no.2 (I think) after 3 iterations. I tried different velocities with the same rpm, but the same is occurring if I decrease the velocity of the inlet.

What is the error when increasing the timestep an indication of?

Thanks

[ghorrocks]

If you cannot increase the time step then your model is not stable enough to allow it. But your model is straight forward and I see nothing which should make it unstable. I bet your mesh is poor quality to cause this.

Can you post some image of your mesh? Especially the mesh around the blades and the transition from the rotating to the stationary domains.

[miquiita]

This is the mesh I had with the code I uploaded.

Thanks

[ghorrocks]

I see a few problems with your mesh:

* A big jump in mesh size from the stationary domain to the rotating domain
* Far too coarse a mesh on the blade
* You appear to have square leading and trailing edges. This is going to cause problems - these are going to shed vortices and therefore a steady state solution will not exist (and this is exactly what you are seeing)

[miquiita]

Hi I looked at the mesh again after posting it to you. I tried to make the mesh less coarse with inflation on the rotating part, domain. I have also fixed the blade so they are less coarse. How fine is the mesh on the blade necessary to be?

Alos "You appear to have square leading and trailing edges. This is going to cause problems - these are going to shed vortices and therefore a steady state solution will not exist (and this is exactly what you are seeing)"

Is this what you seeing on the blade edges? Should I then create inflations or sweap?

thanks

[ghorrocks]

Can you post an image of the cross section profile of your blades? Also include the inflation layers you are using around the blades.

[miquiita]

Yes I can,

if I have a better mesh would that really shorten the solution time? because it takes so long with the mesh to be created.

Here are the pictures of the mesh I created.

I did sizing options and the inflation on the rotor just. On face sizing and then body sizing on the rotor and then the domain around the rotor, smaller cylinder domain.

But running the model I get the message:

| ERROR #001100247 has occurred in subroutine . |
| Message: |
| |
| The solver is unable to continue because of licensing problems. |
| |
| A license for the following capability level could not be checked |
| out: |
| |
| ANSYS CFX Solver (> 512K Nodes) + Licensed Models |
| |
| Please carefully examine the error message output above and check |
| that: |
| |
| 1) The license server is specified correctly and is running. |
| |
| 2) An appropriate license is available for checking out. |
| |
| These problems can be checked using the ANSYS Client ANSLIC_ADMIN |
| utility. For further troubleshooting information please consult |
| ANSYS, Inc. Licensing Guide. |
+-------------------------------------------------------------------

Which means, I think, I have a too fine mesh? For my licence?

[ghorrocks]

The whole point of node limited licenses like this is to stop you from doing real work. So it is not a surprise that when you start trying to do an accurate simulation you run into the node limited license restriction.

So you will need to be very careful about your mesh refinement. Only refine mesh where you really need to. So do a careful sensitivity study to determine where it is needed.

I have uploaded an image which shows the square ends I am talking about. Are you sure your blades look like this? Square ends are always going to shed vorticies and that is always going to make things hard.

And another suggestion: This thing has 3 blades. So why not model it as a single blade with periodic boundary conditions. This would simplify your simulation immensely. Have a look at the CFX tutorials for how to do this.