Problem at the interface in CFX

kwg · October 15, 2014, 08:28

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

ghorrocks · October 15, 2014, 18:14

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

kwg · October 16, 2014, 04:59

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..

ghorrocks · October 16, 2014, 06:32

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?

kwg · October 16, 2014, 06:58

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.

ghorrocks · October 16, 2014, 19:19

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

kwg · October 17, 2014, 05:39

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.

ghorrocks · October 17, 2014, 06:59

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.

kwg · October 17, 2014, 08:07

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..

ghorrocks · October 18, 2014, 04:00

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.

Similar Threads
Thread	Thread Starter	Forum	Replies	Last Post
convergenceof natural convection prob. in cfx	cpkewat	CFX	15	January 31, 2014 07:29
CFX parallel hp MPI problem	fluidmechanics	CFX	5	June 19, 2013 20:05
Problem Importing Geometry ProE to CFX	fatb0y	CFX	3	January 14, 2012 20:42
CFX Casting problem: Can it be done all in one?	jfasl	CFX	1	September 14, 2010 04:14
CFX GGI Interface Error (non-overlapping)	surge519	CFX	1	August 3, 2009 19:54

October 15, 2014, 18:14		#2
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,871 Rep Power: 144	Can you show on your images what the problem is? Also please show your full domain and the flow path from inlet to outlet.

October 16, 2014, 06:32		#4
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,871 Rep Power: 144	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?

October 16, 2014, 19:19		#6
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,871 Rep Power: 144	The tet mesh in image 007.png looks pretty coarse. You will probably have to refine that.

October 17, 2014, 06:59		#8
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,871 Rep Power: 144	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.

October 18, 2014, 04:00		#10
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,871 Rep Power: 144	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.