How to setup mixing plane interface in STAR-CCM+
Hello fellow CFDians,
I am currently trying to create a case with a MFR. Basically it is a blower in a windcanal. There is a non-rotating domain before the blower and one after it. There is no need for a periodicity of the blower as it is completely meshed and implemented. The interface boundaries have similar but are not conform. I use the segregated flow solver and it is an incompressible/isotherm case.
So far I ran a frozen-rotor case which worked fine and now I want to run a case with a mixing plane. For this tried the following combinations:
1. only an indirect interface with mixing plane
2. both an in-place internal interface and an indirect mixing plane
With option 1. The case runs but there is basicall no pressure rise through the blower domain and inlet and outlet mass flow do not match. When I try to set up that case with a start-solution from the frozen rotor (just an in-place interface) it seems, that the mixing plane is working (I checked the interfaces by plotting the velocity on it and it shows me the circumferential average distribution). But the problem is, that this distribution has no effect on the domain as if it was not connected. So even after 800 iterations the solution is basically the same as it was when the calculation started.
When I try to set up option 2 I get an error message when I try to start the simulation or initialize the solution:
SIGSEGV: memory access exception:
In: [Machine::main, SolverManager::initialize, IndirectBoundaryInterfaceSolver::Initializing solution]
Signal: SIGSEGV: memory access exception
error: Server Error
So I assume I did it wrong (first I created the in-place interface then the indirect. each from the same boundaries).
Any ideas what I am doing wrong? Next thing I am going to try is a set up with the coupled solver just to see if it works then. Although the manual said that you only need the coupled solver if you want an explicid interface.
Thanks for any help!
EDIT: Option 1 seems to work somewhat better, but I cannot be sure until it ran a couple hundred iterations.
No replies? Well then I'll have to do that myself!! :p
What was the last step? Ah right I tried it with the coupled solver...This did not work either. Now I think I know what the problem was:
My setup had a non-matching Interface for the mixing plane after the rotor. The first side in the rotor-domain was a full circle while the other side was five separate surfaces divided by the stator-holding-beams (don't know the correct word for it now...basically just obstructions behind the blower). With this setup I could not get a decent solution with consistent mass flows after the rotor-domain. This was no problem for the in-place-interface/frozen rotor. I even compared the solutions from that with a calculation I made with the same mesh in cfx: very similar (if not equal) results. :cool:
What I did to make it work was that I introduced another interface boundary between rotor and stator. For this I took two layers of cells from the rotor-domain and separated them into a new domain with ICEM...Fixed everything up with new shells and voila: now I still have the non-matching interface, but I have it as a in-place interface now. The other conformal boundary between the rotor and in-place interface I used for theindirect/mixing plane inteface. This works very well with the coupled solver. And I also got it to run with the segragated solver. :D
Maybe it is an obvious flaw in my mesh but in my defense the frozen rotor worked initially without a problem. In the end the non-matching interface still exists but as a working in-place interface. Unfortunately it is not an option to remesh the rotor and stator to fix this as the mesh is pre-set.
Finallly in short:
Rotor |Mixing Plane| Stator
Rotor |Mixing Plane| Two layers of Cells |In-Place| Stator
--mrjonezz (edited: sorry used my nickname from different forum)
Having a similar issue. I have a standard internal interface (In-Place) connecting the fluid around the fan to the outlet duct region.
I have added a second mixing plane interface at the same point where the fan fluid connects tot he outlet duct region.
I am measuring the velocity profile downstream but the effects of the stationary rotor are still apparent in the flow. There doesn't appear to be any mixing happening at the mixing plane upstream.
I am using segregated & constant density.
Got a reply from STAR CCM+ help desk. We should only have one interface as you have suggested in your option 1 so this has got me to the point of having a working mixing plane. Thanks.
I now have a mass flow inconsistency between inlet and outlet also. I will try your method of moving the mixing plane away from the rotating region interface.
|All times are GMT -4. The time now is 09:02.|