Problem at the interface in CFX
 

Hi,

I am simulating a (static) guide vane plus some ducting. Some weird things seem to occur at the interface. I am using a stage interface (mixing plane) with a GGI mesh connection.

If I look at some random parameter (in the pictures density is plotted) the averaging on most of the interface seems to be fine. However, where the domain is placed there is some uniformity for basically every parameter.
Does anyone have an idea what causes this? Is this something which disappears with running more iterations?

I tried to change the 'pitch change' option from automatic to manually specifying the pitch angles, this didn't make any difference. So the problem doesn't seem to be here.

Thanks in advance for your help,
Koen

Can you show on your images what the problem is? Also please show your full domain and the flow path from inlet to outlet.

The problem is the non uniform region in picture 003. Where I would expect a minimal variation of any parameter at a certain radius. Except from that region the solution seems to be uniform at a certain radius. So I am wondering what causes this non uniform region and since it is located at a point where also the 60 degree domain of the guide vane is placed, I am suspecting it has to do something with the connection between the two domain. However, I cannot figure out what is wrong..

I can see facets in your cross section. This suggests your mesh is very coarse. Can you show a plot of your mesh? Have you done a mesh refinement study?

I have done similar simulations where I did a mesh refinement study. No problems occurred at the interface at that time and the results were good. Now as a start I used the same mesh settings as for those previous studies.

The tet mesh in image 007.png looks pretty coarse. You will probably have to refine that.

I tried to refine the mesh at the interface, but that didn't make any difference.

However, I managed to find a solution to the problem! Before I didn't have an 'Outlet Domain' in TurboGrid. By adding this outlet domain to the mesh the problem was solved. Now the conditions at the interface look uniform in the circumferential direction (see picture 008). However, I don't really understand why this solved the problem. Since the outlet was close to the trailing edge of the blade, I thought I didn't need an outlet domain. Do you know what is the function of this domain?

I agree that the mesh still looks relatively coarse. I will perform a sensitivity analysis on this, but the problem at the interface seems to be solved.

You have not shown us the full geometry you are modelling (at least I don't think you have) so I cannot comment. You will need to show the full geometry.

See picture 009 and 010 for the full geometry.

Initially I created a mesh in TurboGrid without an 'Outlet Domain', picture 011. Now what I did is I moved the outlet a little bit inwards, so that I could create an 'Outlet Domain' in the mesh, picture 012. That solved the problem, but I don't understand why..

When you have the outlet so close to the blade I would expect the wake of the blade to go to the outlet. This will cause convergence difficulties. When you put in a GGI before the outlet it diffuses the wake (especially with some frame change options which do stage averaging) and reduces the problem.

But it is bad practise to put the outlet so close. You need it further downstream for reliable convergence and accuracy.