CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > CFX

Frozen Rotor 1:1 Mesh Connection

Register Blogs Members List Search Today's Posts Mark Forums Read

Reply
 
LinkBack Thread Tools Display Modes
Old   January 25, 2013, 13:21
Default Frozen Rotor 1:1 Mesh Connection
  #1
New Member
 
Peter Harley
Join Date: Jan 2013
Posts: 3
Rep Power: 4
pharley is on a distinguished road
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
pharley is offline   Reply With Quote

Old   January 28, 2013, 12:01
Default
  #2
Senior Member
 
Christoph
Join Date: May 2011
Location: Germany
Posts: 182
Rep Power: 9
energy382 is on a distinguished road
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?
energy382 is offline   Reply With Quote

Old   January 30, 2013, 08:12
Default
  #3
New Member
 
Peter Harley
Join Date: Jan 2013
Posts: 3
Rep Power: 4
pharley is on a distinguished road
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.
pharley is offline   Reply With Quote

Old   January 30, 2013, 17:48
Default
  #4
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,652
Rep Power: 84
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
Quote:
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.
This is not correct, you have misinterprested the comments. You can only use a GGI to connect domains if there is relative motion between the domains - such as rotation. You can use either a GGI or a 1:1 if both domains share the same motion.

Quote:
it must be remembered that the ANSYS 'Alternative Rotation Model' should be used which removes the centrifugal and Coriolis forces from the equations.
This comment is also wrong. The alternative rotation model includes centrifugal and coriolis forces, just the advection and transient terms are doen in the absolute frame not the rotating frame. The alternative rotation model does not model a domain which is not rotating - a stationary domain does that.
ghorrocks is offline   Reply With Quote

Old   January 31, 2013, 09:44
Default
  #5
New Member
 
Peter Harley
Join Date: Jan 2013
Posts: 3
Rep Power: 4
pharley is on a distinguished road
Quote:
Originally Posted by ghorrocks View Post
This is not correct, you have misinterprested the comments. You can only use a GGI to connect domains if there is relative motion between the domains - such as rotation. You can use either a GGI or a 1:1 if both domains share the same motion.
No I have not misinterpreted, it is no longer possible to have 1:1 mesh connections between fluid-fluid interfaces regardless of their relative motion. Please find the transcript with ANSYS below:

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:
Originally Posted by ghorrocks View Post
This comment is also wrong. The alternative rotation model includes centrifugal and coriolis forces, just the advection and transient terms are doen in the absolute frame not the rotating frame. The alternative rotation model does not model a domain which is not rotating - a stationary domain does that.
It is the advection term in the momentum equations normal to the axis of rotation, which if carried out using the relative velocity introduces forces equivalent to centrifugal. The Navier-Stokes equations do not contain a centrifugal force, this is induced as a result of using a relative frame of reference. As well as this there is a modification to the Coriolis source term. The 'Alternate Rotation Model' is used when you want to avoid using a frame change model at an interface, such as the 'frozen rotor' model.
pharley is offline   Reply With Quote

Old   January 31, 2013, 17:15
Default
  #6
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,652
Rep Power: 84
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
Quote:
No I have not misinterpreted, it is no longer possible to have 1:1 mesh connections between fluid-fluid interfaces regardless of their relative motion.
I see. Very strange. As you can see this is new behaviour for the current version of CFX. All previous versions of CFX support 1:1 interfaces between fluid regions.

Quote:
The 'Alternate Rotation Model' is used when you want to avoid using a frame change model at an interface, such as the 'frozen rotor' model.
No (at least by my understanding ). The alternative rotation model is best used when the domain is rotating but the flow is close to not rotating in the absolute frame. Then the terms are calculated in the absolute frame to reduce round off error. The same terms are calculated and nothing is neglected, it is just which frame of reference they are calculated in. So the alternative rotation model cannot be used to avoid frame changes at interfaces.
ghorrocks is offline   Reply With Quote

Reply

Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
[ICEM] Generating Mesh for STL Car in Windtunnel Simulation tommymoose ANSYS Meshing & Geometry 48 April 15, 2013 04:24
Add Mesh Layers doesnt work on the whole surface Kryo OpenFOAM Native Meshers: snappyHexMesh and Others 8 September 13, 2012 09:28
Layers:problem with curvature giulio.topazio OpenFOAM Native Meshers: snappyHexMesh and Others 10 August 22, 2012 09:03
fluent add additional zones for the mesh file SSL FLUENT 2 January 26, 2008 12:55
basic of mesh refinement arya CFX 4 June 19, 2007 12:21


All times are GMT -4. The time now is 12:30.