sliding mesh problem in CFX
 

Hi All,

There is a tutorial in Fluent "Tutorial 11: Using Sliding Meshes " 2D Tutorial. In fluent problem Fluid phase Velosity (which is given in Fluent around y= -Vx) imposeed under Setup => Cell Zone Conditions.

I want to do same in CFX but i have not foung Fluid Translation in CFX. How can i do it? CFX just have "Rotaion" and stationary" option in "domain"option.

I dont want to give rotaion brcause i am working on airfoil.

Please let me know.

Thank you,

To do anything but rotation you need to use general moving mesh. Translating mesh is meant to be a beta feature but I have never used it and cannot guarantee it works - talk to CFX support if this is of interest.

Saima,

Did you succeed to translate the mesh?

I am looking into almost the same problem.

Saima? did u solve it?

These posts are 4 years old, it is unlikely you will get any response except from the tragics like me :)

But my post from 4 years ago still stands - use moving mesh to do it.

Glenn,

In all of the posts that there has been some issue with translational mesh motion you said that it is possible and yes it is. But there is one problem.
you see in my case there are two domains, one stationary, the other one is supposed to translate(not rotating, translating)
for the time steps that the interfaces of the two domains are not overlapping 100%, the solver assumes there is a wall for the non-overlapping area. Unlike the "transient rotor stator" interface. It seems that CFX can only do the sliding mesh for rotational cases not translational cases.
Now do you have any knowledge that this problem can be overcome. Maybe I can use CFX to implement translationan sliding mesh??

Thanks,

Ali

This interface connecting a domain with moving mesh (for translational motion) to a stationary domain works fine. You need to use transient rotor/stator interface setting.

CFX can handle translational interfaces fine. It is not restricted to rotational interfaces.

Are you sure? Have you done it yourself? Because when I do that I receive an error. Also When I specify transient rotor-stator interface it asks for the axis of rotation.

We are sure. Have done it thousands of times. What error are you getting? What kind of behavior do you want for non-overlapping interfaces?

This is the error that I get.

+--------------------------------------------------------------------+
| ERROR #004100018 has occurred in subroutine FINMES.|
| Message: |
| Fatal overflow in linear solver. |
+--------------------------------------------------------------------+

Here I also have attached the CCL. Please take a look.

Thanks,

# State file created: 2014/04/29 15:32:12
# CFX-15.0 build 2013.10.10-08.49-130242

FLOW: Flow Analysis 1
SOLUTION UNITS:
Angle Units = [rad]
Length Units = [m]
Mass Units = [kg]
Solid Angle Units = [sr]
Temperature Units = [K]
Time Units = [s]
END
ANALYSIS TYPE:
Option = Transient
EXTERNAL SOLVER COUPLING:
Option = None
END
INITIAL TIME:
Option = Automatic with Value
Time = 0 [s]
END
TIME DURATION:
Option = Total Time
Total Time = 1.5 [s]
END
TIME STEPS:
Option = Timesteps
Timesteps = 0.005 [s]
END
END
DOMAIN: Default Domain
Coord Frame = Coord 0
Domain Type = Fluid
Location = BODY
BOUNDARY: Domain Interface 1 Side 1
Boundary Type = INTERFACE
Location = PER_1
BOUNDARY CONDITIONS:
MASS AND MOMENTUM:
Option = Conservative Interface Flux
END
MESH MOTION:
Option = Conservative Interface Flux
END
TURBULENCE:
Option = Conservative Interface Flux
END
END
END
BOUNDARY: Domain Interface 1 Side 2
Boundary Type = INTERFACE
Location = PER_2
BOUNDARY CONDITIONS:
MASS AND MOMENTUM:
Option = Conservative Interface Flux
END
MESH MOTION:
Option = Conservative Interface Flux
END
TURBULENCE:
Option = Conservative Interface Flux
END
END
END
BOUNDARY: Domain Interface 2 Side 1
Boundary Type = INTERFACE
Location = INLET
BOUNDARY CONDITIONS:
MASS AND MOMENTUM:
Option = Conservative Interface Flux
END
MESH MOTION:
Option = Unspecified
END
TURBULENCE:
Option = Conservative Interface Flux
END
END
END
BOUNDARY: out
Boundary Type = OUTLET
Location = OUTLER
BOUNDARY CONDITIONS:
FLOW REGIME:
Option = Subsonic
END
MASS AND MOMENTUM:
Option = Static Pressure
Relative Pressure = 0 [Pa]
END
MESH MOTION:
Option = Stationary
END
END
END
BOUNDARY: pressure surface
Boundary Type = WALL
Location = PS
BOUNDARY CONDITIONS:
MASS AND MOMENTUM:
Option = No Slip Wall
Wall Velocity Relative To = Mesh Motion
END
MESH MOTION:
Option = Stationary
END
WALL ROUGHNESS:
Option = Smooth Wall
END
END
END
BOUNDARY: suction suface
Boundary Type = WALL
Location = SS
BOUNDARY CONDITIONS:
MASS AND MOMENTUM:
Option = No Slip Wall
Wall Velocity Relative To = Mesh Motion
END
MESH MOTION:
Option = Stationary
END
WALL ROUGHNESS:
Option = Smooth Wall
END
END
END
BOUNDARY: symmetric back
Boundary Type = SYMMETRY
Location = SYM1
BOUNDARY CONDITIONS:
MESH MOTION:
Option = Unspecified
END
END
END
BOUNDARY: symmetric front
Boundary Type = SYMMETRY
Location = SYM2
BOUNDARY CONDITIONS:
MESH MOTION:
Option = Unspecified
END
END
END
DOMAIN MODELS:
BUOYANCY MODEL:
Option = Non Buoyant
END
DOMAIN MOTION:
Option = Stationary
END
MESH DEFORMATION:
Displacement Relative To = Previous Mesh
Option = Regions of Motion Specified
MESH MOTION MODEL:
Option = Displacement Diffusion
MESH STIFFNESS:
Option = Increase near Small Volumes
Stiffness Model Exponent = 10
REFERENCE VOLUME:
Option = Mean Control Volume
END
END
END
END
REFERENCE PRESSURE:
Reference Pressure = 1 [atm]
END
END
FLUID DEFINITION: Fluid 1
Material = Air at 25 C
Option = Material Library
MORPHOLOGY:
Option = Continuous Fluid
END
END
FLUID MODELS:
COMBUSTION MODEL:
Option = None
END
HEAT TRANSFER MODEL:
Option = None
END
THERMAL RADIATION MODEL:
Option = None
END
TURBULENCE MODEL:
Option = k omega
END
TURBULENT WALL FUNCTIONS:
Option = Automatic
END
END
END
DOMAIN: Domain 1
Coord Frame = Coord 0
Domain Type = Fluid
Location = BODY 2
BOUNDARY: Domain Interface 2 Side 1 1
Boundary Type = INTERFACE
Location = FAM2
BOUNDARY CONDITIONS:
MASS AND MOMENTUM:
Option = Conservative Interface Flux
END
MESH MOTION:
Option = Unspecified
END
TURBULENCE:
Option = Conservative Interface Flux
END
END
END
BOUNDARY: Domain Interface 3 Side 1
Boundary Type = INTERFACE
Location = PER1
BOUNDARY CONDITIONS:
MASS AND MOMENTUM:
Option = Conservative Interface Flux
END
MESH MOTION:
Option = Conservative Interface Flux
END
TURBULENCE:
Option = Conservative Interface Flux
END
END
END
BOUNDARY: Domain Interface 3 Side 2
Boundary Type = INTERFACE
Location = PER2
BOUNDARY CONDITIONS:
MASS AND MOMENTUM:
Option = Conservative Interface Flux
END
MESH MOTION:
Option = Conservative Interface Flux
END
TURBULENCE:
Option = Conservative Interface Flux
END
END
END
BOUNDARY: in
Boundary Type = INLET
Location = FAM1
BOUNDARY CONDITIONS:
FLOW REGIME:
Option = Subsonic
END
MASS AND MOMENTUM:
Option = Cartesian Velocity Components
U = Vinx
V = Viny
W = 0 [m s^-1]
END
MESH MOTION:
Option = Stationary
END
TURBULENCE:
Fractional Intensity = 0.019
Option = Intensity and Auto Compute Length
END
END
END
BOUNDARY: rod 1
Boundary Type = WALL
Location = ROD1,ROD2
BOUNDARY CONDITIONS:
MASS AND MOMENTUM:
Option = No Slip Wall
Wall Velocity Relative To = Mesh Motion
END
MESH MOTION:
Option = Stationary
END
WALL ROUGHNESS:
Option = Smooth Wall
END
END
END
BOUNDARY: sym 1
Boundary Type = SYMMETRY
Location = SYM1 2
BOUNDARY CONDITIONS:
MESH MOTION:
Option = Unspecified
END
END
END
BOUNDARY: sym 2
Boundary Type = SYMMETRY
Location = SYM2 2
BOUNDARY CONDITIONS:
MESH MOTION:
Option = Unspecified
END
END
END
DOMAIN MODELS:
BUOYANCY MODEL:
Option = Non Buoyant
END
DOMAIN MOTION:
Option = Stationary
END
MESH DEFORMATION:
Displacement Relative To = Previous Mesh
Option = Regions of Motion Specified
MESH MOTION MODEL:
Option = Displacement Diffusion
MESH STIFFNESS:
Option = Increase near Small Volumes
Stiffness Model Exponent = 2.0
REFERENCE VOLUME:
Option = Mean Control Volume
END
END
END
END
REFERENCE PRESSURE:
Reference Pressure = 1 [atm]
END
END
FLUID DEFINITION: Fluid 1
Material = Air at 25 C
Option = Material Library
MORPHOLOGY:
Option = Continuous Fluid
END
END
FLUID MODELS:
COMBUSTION MODEL:
Option = None
END
HEAT TRANSFER MODEL:
Option = None
END
THERMAL RADIATION MODEL:
Option = None
END
TURBULENCE MODEL:
Option = k omega
END
TURBULENT WALL FUNCTIONS:
Option = Automatic
END
END
SUBDOMAIN: Subdomain 1
Coord Frame = Coord 0
Location = BODY 2
MESH MOTION:
Option = Specified Displacement
DISPLACEMENT:
Displacement X Component = 00 [m]
Displacement Y Component = 0.1 [m]*Time This Run/1 [s]
Displacement Z Component = 0 [m]
Option = Cartesian Components
END
END
END
END
DOMAIN INTERFACE: Domain Interface 1
Boundary List1 = Domain Interface 1 Side 1
Boundary List2 = Domain Interface 1 Side 2
Interface Type = Fluid Fluid
INTERFACE MODELS:
Option = Translational Periodicity
MASS AND MOMENTUM:
Option = Conservative Interface Flux
MOMENTUM INTERFACE MODEL:
Option = None
END
END
END
MESH CONNECTION:
Option = GGI
END
END
DOMAIN INTERFACE: Domain Interface 2
Boundary List1 = Domain Interface 2 Side 1 1
Boundary List2 = Domain Interface 2 Side 1
Interface Type = Fluid Fluid
INTERFACE MODELS:
Option = General Connection
FRAME CHANGE:
Option = Transient Rotor Stator
END
MASS AND MOMENTUM:
Option = Conservative Interface Flux
MOMENTUM INTERFACE MODEL:
Option = None
END
END
PITCH CHANGE:
Option = Automatic
AXIS DEFINITION:
Option = Coordinate Axis
Rotation Axis = Coord 0.3
END
END
END
MESH CONNECTION:
Option = GGI
END
END
DOMAIN INTERFACE: Domain Interface 3
Boundary List1 = Domain Interface 3 Side 1
Boundary List2 = Domain Interface 3 Side 2
Interface Type = Fluid Fluid
INTERFACE MODELS:
Option = Translational Periodicity
MASS AND MOMENTUM:
Option = Conservative Interface Flux
MOMENTUM INTERFACE MODEL:
Option = None
END
END
END
MESH CONNECTION:
Option = Automatic
END
END
INITIALISATION:
Option = Automatic
INITIAL CONDITIONS:
Velocity Type = Cartesian
CARTESIAN VELOCITY COMPONENTS:
Option = Automatic with Value
U = 3.074848454 [m s^-1]
V = -2.153036289 [m s^-1]
W = 0 [m s^-1]
END
STATIC PRESSURE:
Option = Automatic with Value
Relative Pressure = 20 [Pa]
END
TURBULENCE INITIAL CONDITIONS:
Option = Medium Intensity and Eddy Viscosity Ratio
END
END
END
OUTPUT CONTROL:
MONITOR OBJECTS:
MONITOR BALANCES:
Option = Full
END
MONITOR FORCES:
Option = Full
END
MONITOR PARTICLES:
Option = Full
END
MONITOR RESIDUALS:
Option = Full
END
MONITOR TOTALS:
Option = Full
END
END
RESULTS:
File Compression Level = Default
Option = Standard
END
TRANSIENT RESULTS: Transient Results 1
File Compression Level = Default
Include Mesh = On
Option = Selected Variables
Output Variables List = Absolute Pressure,Courant \
Number,Density,Dynamic Viscosity,Eddy \
Viscosity,Pressure,Velocity,Wall Shear,Velocity u,Velocity w,Velocity \
v,Vorticity X,Vorticity Y,Vorticity Z,Wall Shear X,Wall Shear Y,Wall \
Shear Z,Yplus,Wall Normal Velocity,Total Pressure,Turbulence Eddy \
Dissipation,Turbulence Eddy Frequency,Turbulence Kinetic Energy,Total \
Mesh Displacement X,Total Mesh Displacement Y,Total Mesh Displacement \
Z,Mesh Displacement X,Mesh Displacement Y,Mesh Displacement Z,Mesh \
Velocity X,Mesh Velocity Y,Mesh Velocity Z,Boundary Scale,Boundary \
Distance,Mesh Displacement,Mesh Expansion Factor,Orthogonality \
Angle,Orthogonality Angle Minimum,Orthogonality Factor,Orthogonality \
Factor Minimum
OUTPUT FREQUENCY:
Option = Every Timestep
END
END
TRANSIENT STATISTICS: Transient Statistics 1
Option = Arithmetic Average
Output Variables List = Absolute Pressure,Density,Pressure,Total \
Pressure,Velocity,Velocity Correlation,Vorticity,Yplus,Velocity \
Correlation ww,Vorticity X,Vorticity Y,Vorticity Z,Lighthill Stress \
vw,Lighthill Stress ww,Velocity Correlation uu,Velocity Correlation \
uv,Velocity Correlation uw,Velocity Correlation vv,Velocity \
Correlation vw,Boundary Scale,Dynamic Viscosity,Eddy \
Viscosity,Courant Number,Boundary Distance,Mesh \
Displacement,Orthogonality Factor,Orthogonality Angle \
Minimum,Orthogonality Factor Minimum,Orthogonality Angle,Total Mesh \
Displacement,Total Centroid Displacement,Turbulence Eddy \
Dissipation,Turbulence Eddy Frequency,Turbulence Kinetic Energy,Wall \
Shear
END
END
SOLVER CONTROL:
Turbulence Numerics = High Resolution
ADVECTION SCHEME:
Option = Upwind
END
CONVERGENCE CONTROL:
Maximum Number of Coefficient Loops = 10
Minimum Number of Coefficient Loops = 1
Timescale Control = Coefficient Loops
END
CONVERGENCE CRITERIA:
Residual Target = 0.000001
Residual Type = RMS
END
EQUATION CLASS: continuity
ADVECTION SCHEME:
Option = Upwind
END
END
EQUATION CLASS: ke
ADVECTION SCHEME:
Option = High Resolution
END
END
EQUATION CLASS: momentum
ADVECTION SCHEME:
Option = Upwind
END
END
EQUATION CLASS: tef
ADVECTION SCHEME:
Option = High Resolution
END
END
INTERRUPT CONTROL:
INTERRUPT CONDITION: Interrupt Condition 1
Logical Expression = remeshingcond
Option = Logical Expression
END
END
INTERSECTION CONTROL:
Option = Direct
Permit No Intersection = On
END
TRANSIENT SCHEME:
Option = First Order Backward Euler
END
END
EXPERT PARAMETERS:
degeneracy check tolerance = 1.e-2
tbulk for htc = 298
topology estimate factor = 1.8
vector parallel tolerance = 15
END
END
COMMAND FILE:
Version = 15.0
END

You have a velocity specified inlet with an incompressible fluid, and you have talked about an interface opening and shutting. If fluid is forced to flow in the inlet and it is not connected to the outlet and has nowhere else to go then you will crash with an overflow error.

Glenn,

Thanks but what is your suggestion exactly?
I mean how else I am supposed to define the problem? specify pressure at the inlet and mass flow at the outlet?
why it does not work in this way?

When there is no outlet, you are trying to compress the air. Since you are using incompressible air for the fluid, this wont work.

Either switch to air ideal gas (and you will have to deal with the internal shocks), or put an outlet somewhere in your model.

there is an outlet at the end of second domain. the flow is coming in from the inlet and is supposed to go through the interface and enter the second one and then exit from the outlet in the second domain. Will it work?

From your posts, it seemed that for some period of time, your interfaces are not connect. I assume they start off not connected and slide together to connect, thus allowing flow.

During the time they are not connected, you have the situation I described above, with the inlet not seeing any outlet and you are trying to compress the air.

So, no, the way you have it set up now will not work.

Thanks for the info

you can see the both domains in this picture. The left (tiny) one is supposed to move and the other one is supposed to be stationary. The interfaces are initially 100
% overlapping but after time the overlapping part reduces.
Inlet is "velocity inlet" and "pressure" at the outlet is specified. at the very end of the simulation the areas are still overlapping(maybe about 10%) but the fact is the periodic boundary conditions specified on both domains for top and bottom surfaces and also having TRS interface should prevent that problem that you are saying. Isn't it?

OK this is a bit different than I described.

When are you getting your error? First iteration?

No, it happens after a while. Like maybe after 15 minutes

after 50th timestep

Any suggestions Edmund?

Can you explain what is happening around the 50th time step? I recall you have rod things which are closing up a gap. Is this just before the rods close the gap? An image of what the mesh looks like would help.

Actually I have posted a picture couple of posts back and if you take a look at it you can see that the rods are there only to produce some wakes. They are not closing up a gap.
By 50th time step the domain on left has barely moved. it has displaced only about 0.025m(2.5 cm)

Did you verify that flow is actually moving through the interface in that little bit that did run? Just to verify that it is setup correctly.

But I am beginning to suspect mesh quality.

Here you can see some pictures. I do not know what is causing the problem?
For initial condition I have set the interface frame change type to "none" and you can see that the results are reasonable(the first two pictures). Then I set this solution as initial condition for the transient solution and as you can see in the next two pictures the velocity value goes through the roof.(for transient case the interface type is set to TRS)

any idea why this is happening?

the last two images are taken at the timestep that the solver crashes

This happens when the simulation diverges. To fix this you need to improve the numerical stability. You can do this by some combination of:
* Better quality mesh
* Smaller time steps
* Double precision numerics
* Better initial condition.
* Use first order differencing (but this will compromise the accuracy)

I asked ansys support team to help me with that and they said that Transient-Rotor stator interface model(TRS) will not do the transnational sliding mesh modeling...It only can do the rotational sliding mesh

End of Story

TRS works fine with a translating mesh when the translation is done as a moving mesh. If you are using a translating frame of reference it does not surprise me things don't work - that's why translating frame of reference is not a fully released feature.

Glenn,

Thanks, but I used moving mesh as you said. not moving frame of reference. I have spent over a month struggling with TRS and translational sliding mesh and now I can say with 100% confidence that CFX cannot do that.
especially after I opened a thread in CFX support portal and worked with CFX representative for more than a week. After that he told me explicitly that CFX cannot do that and suggested using a rotational sliding mesh with relatively large radius of rotation instead.

Glenn, If you have done that before and still have a .pre file or the ccl please give it to me somehow so that I can show it to CFX technical support.

Interesting - because I have 100% confidence that is does work (well, at least did work) because I have used it several times. I will admit that the last time I used it was many years ago although I cannot remember exactly which version. The models were a 2-stoke port valve engine using GGIs which open and shut as the piston slides past them and a hydraulic pressure relief valve which cracked open with a translational motion. Both these models were with a previous employer and I no longer have the files available. I think I was doing the 2 stroke engine about 12 years ago and the hydraulic valve about 8 years ago - so a fair way back.

It is possible that this functionality has been broken in recent releases. It would be a shame if it does not work any more.

Glenn, You still can slide a mesh relative to the other one . but you can not use TRS model for the interface between the two grids. that is the issue. TRS is not compatible with translational movement.
For non-overlapping portion it can only uses wall type boundary condition and you can not change it to any other type of boundary.
In the picture you can see that the non-overlapping portion at the end of the simulation is treating as a wall

I see, we might be talking to crossed purposes here.

The image you shows has the interface functioning perfectly - so it looks like a TRS interface is working fine. You issue seems to be the wall which is generated in the non-overlapping portion. In my case of port valve engines the non-overlapping section indeed was a wall so the default behaviour is correct for my application.

But would I be correct in saying that you are trying a model with translational periodicity, and you want this interface section to match up with the flow on the other side of the periodic condition, presumably at the top of the domain?

This is what TRS is good for. Aparently it is not working with translational movement of the domains

OK, I think we have made some progress. TRS works fine for matching up the mesh interfaces as long as you are happy for the non-overlapping section to be a wall. If you want the non-overlapping section to map around to the other side of the domain (as it does in rotational cases) then this is not supported.

Now I understand what you are talking about the recommendation is simple - rather than modelling a single periodic unit and expecting the interface to handle the non-overlapping section, you model two periodic units. The top and bottom of the model is rubbish as an artificial wall is generated, but the middle section away from the non-overlapping section should be fine. If you find your results are affected by proximity to the non-overlapping region then model 3 or more periodic units until the effect is small enough to ignore.

This solution is not ideal as it doubles the size of the simulation, but at least you can run it without modelling the whole thing.

I am using a transient rotor stator interface between one rotating domain and one stationary domain. For this kind of an interface, if I am not wrong, I think the non overlapped regions should behave like a wall.

However in my case, the flow occurs even through the non overlapped regions. The simulation is a transient simulation and the overlap area changes with time. What could be going wrong ?

I think you have to set this behaviour manually.

Thanks for replying Antanas

How do I set it manually ?

Inside properties of interface side that is not fully overlapped. There is nonoverlap conditions tab.