|
[Sponsors] |
January 25, 2013, 12:21 |
Frozen Rotor 1:1 Mesh Connection
|
#1 |
New Member
Peter Harley
Join Date: Jan 2013
Posts: 3
Rep Power: 13 |
I am creating a model based on a centrifugal compressor. I have generated the geometry using BladeGen, and the mesh using TurboGrid. It is a single passage model so has periodics.
I have an INblock, a main blade Passage, and an OUTblock. The complete passage was meshed in TurboGrid so 1:1 connectivity exists between all blocks. I also have 1:1 on the periodics. I import this to CFX-Pre using the Turbo mode function and create a stationary domain for the INblock, a rotating domain for the Passage, and a stationary domain for the OUTblock, and frozen rotor interfaces between them. The periodics are set up automatically. When checking the interface mesh connections between the INblock and Passage, and the Passage and OUTblock, I find that the Mesh Connection is GGI. When I select the drop down list there are no other options. I manually added connectivity at the interfaces, and it does not complain about the 1:1 here, but I still cannot select it as a mesh connection. I glued the meshes together, still cannot select 1:1. I tried to make all three domains rotate and select 'None' as the interfaces and use the alternative rotation model for the stationary domains. Am I missing something obvious here? Is it possible to have a 1:1 mesh connection with a frozen rotor interface? I have started the simulation in Solver to check and it is definitely only recognising a GGI. Peter |
|
January 28, 2013, 11:01 |
|
#2 |
Senior Member
Christoph
Join Date: May 2011
Location: Germany
Posts: 182
Rep Power: 18 |
usually, I use just one interface for a single blade simulation. Stationary inflow domain, frozen rotor interface, rotating impeller and rotating outflow (counter-rotating).
You can adjust your mesh match tolerance in CFX Pre-> edit/options/mesh Turbogrid can't deal with radius zero as I know. So you have a sloped interface (frozen rotor). Am I right? |
|
January 30, 2013, 07:12 |
|
#3 |
New Member
Peter Harley
Join Date: Jan 2013
Posts: 3
Rep Power: 13 |
After contacting ANSYS it has become clear that one cannot add a 1:1 mesh connection between domains, instead the GGI mesh connection must be used.
Also with regard to having an outlet domain rotating (which is stationary in reality), it must be remembered that the ANSYS 'Alternative Rotation Model' should be used which removes the centrifugal and Coriolis forces from the equations. So the answer to my question is, it can't be done. |
|
January 30, 2013, 16:48 |
|
#4 | ||
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,826
Rep Power: 144 |
Quote:
Quote:
|
|||
January 31, 2013, 08:44 |
|
#5 | ||
New Member
Peter Harley
Join Date: Jan 2013
Posts: 3
Rep Power: 13 |
Quote:
ME: I am creating a model based on a centrifugal compressor. I have generated the geometry using BladeGen, and the mesh using TurboGrid. It is a single passage model so has periodics. I have an INblock, a main blade Passage, and an OUTblock. The complete passage was meshed in TurboGrid using the ATM Optimized method so 1:1 connectivity exists between all blocks. I also have 1:1 on the periodics. I import this to CFX-Pre using the Turbo mode function and create a stationary domain for the INblock, a rotating domain for the Passage, and a stationary domain for the OUTblock, and frozen rotor interfaces between them. The periodics are set up automatically. When checking the interface mesh connections between the INblock and Passage, and the Passage and OUTblock, I find that the Mesh Connection is GGI. When I select the drop down list there are no other options. I manually added connectivity at the interfaces, and it does not complain about the 1:1 here, but I still cannot select it as a mesh connection. I glued the meshes together, still cannot select 1:1. I tried to make all three domains rotate and select 'None' as the interfaces and use the alternative rotation model for the stationary domains and still cannot select 1:1. Am I missing something obvious here? Is it possible to have a 1:1 mesh connection with a frozen rotor interface or even a fluid fluid interface? I have started the simulation in Solver to check the mesh connections and it is definitely only recognising a GGI. ANSYS: The rotor-stator interfaces are always treated as a GGI interface, in CFX. There is no other option. This is because the solver can correctly account for the flux conservation, which is not done when using the 1:1 interface. ME: Is it ever possible to create a 1:1 mesh connection between 2 domains? I have also tried to set this up by exporting from TurboGrid the separate domain files, importing this is CFX-Pre and keeping all domains stationary and still I cannot select 1:1. Is this a limitation of the CFX solver as I do not see a reason why flux conservation cannot be carried out across an interface with 1:1 connectivity? Is this an inherent part of the CFX code? The ANSYS manual 5.4.4 states the following: "Domain interfaces that use GGI connections are a very powerful and flexible mesh connection method, but they do require some additional computational effort and memory, and may introduce numerical inaccuracy compared to an equivalent computation that does not use GGI connections. For these reasons, you should use GGI connections wisely and sparingly." One reads this and immediately thinks that a 1:1 mesh connection should be used instead. The ANSYS manual Chapter 3 states the following: "Multiple Frames of Reference (MFR) allows the analysis of situations involving domains that are rotating relative to one another. For CFX, this feature focuses on the investigation of rotor/stator interaction for rotating machinery. Because MFR is based on the GGI technology, the most appropriate meshing style may be used for each component in the analysis." So my questions are: If the frozen rotor interface MUST use a GGI mesh connection, but the mesh is actually 1:1, how much if any interpolation is carried out by the Solver? Is this the most efficient interface for such an analysis? Is it even worth while creating a 1:1 mesh across any fluid-fluid interface if a GGI is always applied? ANSYS: You can create a 1:1 to interface if you are connecting stationary to stationary (or rotating to rotating) domains, this only happens when you have generated a meshes which are 1:1 connected. When importing a single component mesh with inlet, passage and outlet regions, from TG; you can just set them up as a single domain. At which point you dont need any domains interface as the meshes are 1:1 connected. As said earlier, for rotor-stator type interfaces the option available is only GGI. The GGI option is also available to other interface types, as well. The reason for using GGI interface is it does additional flux conservation, as compared to 1:1 interface, which does not explicitly account for the flux conservation, so at convergence the flux will be get conserved, implicitly. In CFX solver, the 1:1 option is removed, so the flux conservation can be correctly accounted for each timestep and not just at the end of simulation. So for your questions: If the frozen rotor interface MUST use a GGI mesh connection, but the mesh is actually 1:1, how much if any interpolation is carried out by the Solver? Is this the most efficient interface for such an analysis? answer: The GGI interface has been well validated over various cases and fine tuned over many CFX releases. Currently this is the default. Using 1:1 mesh will reduce the interpolation errors for the local variables profiles, as compared to many elements connecting to 1 elemenet. As for efficiency, the time penalty is small when using GGI, typically less than 5%. But the flux conservation helps in quicker convergence and lesser number of interations. If the mesh mismatch is large then you can have significant interpolation errors, so it is recommended to have mismatch not greater than 1:3 across the interface. Is it even worth while creating a 1:1 mesh across any fluid-fluid interface if a GGI is always applied? Answer: It is not a requirement to generate 1:1 meshes. Typically generating mismatched meshes means reducing the compexity of mesh generation and spend lesser time meshing the cases. ME: So it is possible to have 1:1 between rotating domains with the same rotational velocity? I am now using the TurboGrid mesh that has an Inlet, Passage, and Outlet all in one mesh (definitely 1:1), creating 3 rotating domains (all with the same rotational velocity) each with the interface model set to 'None', and still I cannot select 1:1. The inlet and outlet domains contain no features. At this time I have not selected the 'Alternate Rotation Model' although I know I have to use this to remove the centrifugal and Coriolis forces. Is there something else I should be doing? ANSYS: Seems like the behaviour of CFX Pre has been changed from the previous versions and now its only possible to set GGI for rotating domains. Another option for you would be solve the 3 meshes, as a single domain, then you will not need to setup the interface. I'm checking this with our developers and will get back to you if its possible to change it. You will need to switch on the Alternate rotation model, to reduce the numerical errors in the stationary parts. ANSYS: The GGI specification has been traced to be a software bug. It is planned to be fixed for the next release v14.5. So surrently the only option would be use GGI interfaces. ME: Ok at least we have an answer now, however I have already tried to do this in v14.5 as well, and the same problem exists. Is there a service pack to be released for 14.5? If so can you comment on the release date of a future version that will have this corrected? ANSYS: Based on further investigation, the only option available in CFX to connect two meshes in different fuild domains is via GGI. For 1:1 meshes across the regions, the condition will use the 1:1 connection information to generate the control surface. If you want 1:1 to connection between two meshes then they need to be in the same domain. As such this method will not change in the current or the future versions of the software. Quote:
|
|||
January 31, 2013, 16:15 |
|
#6 | ||
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,826
Rep Power: 144 |
Quote:
Quote:
|
|||
Thread Tools | Search this Thread |
Display Modes | |
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
[snappyHexMesh] Add Mesh Layers doesnt work on the whole surface | Kryo | OpenFOAM Meshing & Mesh Conversion | 13 | February 17, 2022 07:34 |
[ICEM] Generating Mesh for STL Car in Windtunnel Simulation | tommymoose | ANSYS Meshing & Geometry | 48 | April 15, 2013 04:24 |
[snappyHexMesh] Layers:problem with curvature | giulio.topazio | OpenFOAM Meshing & Mesh Conversion | 10 | August 22, 2012 09:03 |
fluent add additional zones for the mesh file | SSL | FLUENT | 2 | January 26, 2008 11:55 |
basic of mesh refinement | arya | CFX | 4 | June 19, 2007 12:21 |