Question about adaptive timestepping
 

Im running a transient simulation with adaptive timestepping aiming for 3-5 coeff loops. The thing is that after 2 days of running the timestep size is around 1E-5 sec, which due to the project time contrains makes it impossible to carry on.

My question is what are the consecuenses of using simply a timestep of 1E-2 instead from the beggining?

Any other alternative solution is highly appreciated.

If you use a time step far larger than recommended then either it will not converge or your results are likely to be rubbish. If you could use a far larger time step than it recommends then why would this be the recommended way of setting time step?

You options are:
* The time step is small because it is having problems converging. So why is it having problems converging? Mesh quality is a key factor here, improvements in mesh quality will assist convergence and allow bigger time steps and therefore faster simulations.
* Get more parallel licenses and a bigger cluster. CFD is extremely computer intensive and there is no way around it. Serious CFD is done on seriously big computer clusters.

Also, besides mesh quality, mesh size makes a large difference as well. you can use a larger time step with a larger mesh.

So basically refining the mesh in the zones where the poorest quality elements are, and make it "coarser" on the zones where mesh quality is not s problem?

Sent from my XT1021 using CFD Online Forum mobile app

Mesh quality and mesh size are not interchangeable. They are different things and have very different effects.

If you refine an area of poor quality mesh you are likely to just get small poor quality elements which will slow convergence. So unless refining the mesh allows you to improve the mesh quality it will not speed things up.

So the mesh size is set by your accuracy requirements. Then you do the best quality mesh you can using that size to get the fastest and most reliable convergence possible.

Im confussed then. All i have read related to improving mesh quality says basically the same: use proper sizing and inflation in every place that is required.

That being said, if you have your elements sizes fixed in your domain (and inflation where it is required), how can you improve mesh quality without changing sizing settings?

Sent from my XT1021 using CFD Online Forum mobile app

Mesh quality is things like aspect ratio, orthogonality, expansion ratio.

Mesh size is... well, just mesh size. The size can be different in different directions (eg inflation layers have different tangential and normal sizes).

You are correct in that when you adjust mesh quality you often change mesh size a bit and vice versa. But they are different parameters with different results.

There is many ways of changing mesh quality with minimal effects on size. These include:
* tet vs hex meshes
* mesh smoothing
* expansion ratio, transitions from inflation layers to bulk mesh

i have tried all of those methods and the best quality ive got is:

skewness: 0,89
orth quality: 0,16
max aspect ratio: 16

According to the doccumentation these are in the "acceptable" range, but i dont know how to improve them more :/

Different simulations have different mesh quality requirements. A incompressible low Reynolds number simulation is tolerant of very poor mesh. Surface tension and shock waves are two examples of models which have a far more stringent mesh quality requirement. So the documentation is just a guide here, your specific case may be quite different.

How does that mesh run?

It runs fine judging by my monitors but my huge problem is the tiny timestep size due to adaptive timestepping

The tiny time step is the solution, not the problem. You have to find a way of making the run time manageable despite the small time step. This is why ANSYS has done years of work to get CFX a parallel good speed up to thousands of processors - CFD requires seriously big hardware to do complex simulations.

Can you post an image of what you are modelling, an image of the flow and mesh in the problem region and your CCL?

how can i post my CCL?

The CCL should be just a small text file. Posting it as an attachment is preferred, but copy/paste into the forum text is OK as well.

As you may remember from other posts, im simulating a wind machine which is being used for frost protection on a vineyard. My geometry is the following:

-Giant "cube" of air of 200 mts long x 50 mts wide x 50 mts high
-inclined cilinder 2 mts diameter used as a general momentum source
-around 70 "squared cilinders" near the ground, each representing a row of vinetrees
-additional geometry behind the general momentum source cilinder, wich represents the engine (btw the engine is JUST a geometrical entity, no combustion or anything)

For more clarity (and the meshing) see pictures attached.

CCL (I cannot attach the file due to file size restrictions)


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 = 37.5 [s]
END
TIME STEPS:
First Update Time = 0.0 [s]
Initial Timestep = 1E-4 [s]
Option = Adaptive
Timestep Update Frequency = 1
TIMESTEP ADAPTION:
Maximum Timestep = 20 [s]
Minimum Timestep = 1E-20 [s]
Option = Number of Coefficient Loops
Target Maximum Coefficient Loops = 5
Target Minimum Coefficient Loops = 3
Timestep Decrease Factor = 0.8
Timestep Increase Factor = 1.06
END
END
END
DOMAIN: estructura_motor
Coord Frame = Coord 0
Domain Type = Solid
Location = estructura_motor
BOUNDARY: Default Fluid Solid Interface Side 1 1
Boundary Type = INTERFACE
Location = \
F2065.2064,F2066.2064,F2067.2064,F2068.2064,F2069. 2064,F2070.2064,F20\
71.2064,F2072.2064,F2073.2064,F2074.2064,F2075.206 4,F2076.2064,F2077.\
2064,F2078.2064
END
DOMAIN MODELS:
DOMAIN MOTION:
Angular Velocity = 0.2 [rev min^-1]
Option = Rotating
AXIS DEFINITION:
Option = Coordinate Axis
Rotation Axis = Coord 1.2
END
END
MESH DEFORMATION:
Option = None
END
END
INITIALISATION:
Coord Frame = Coord 0
Frame Type = Rotating
Option = Automatic
END
SOLID DEFINITION: motor
Material = Aluminium
Option = Material Library
MORPHOLOGY:
Option = Continuous Solid
END
END
SOLID MODELS:
HEAT TRANSFER MODEL:
Option = None
END
THERMAL RADIATION MODEL:
Option = None
END
END
END
DOMAIN: parras
Coord Frame = Coord 0
Domain Type = Porous
Location = parras
BOUNDARY: Default Fluid Porous Interface Side 1 1
Boundary Type = INTERFACE


BOUNDARY CONDITIONS:
HEAT TRANSFER:
Option = Conservative Interface Flux
END
MASS AND MOMENTUM:
Option = Conservative Interface Flux
END
TURBULENCE:
Option = Conservative Interface Flux
END
END
END
BOUNDARY: parras Default
Boundary Type = WALL

BOUNDARY CONDITIONS:
HEAT TRANSFER:
Option = Adiabatic
END
MASS AND MOMENTUM:
Option = No Slip Wall
END
WALL ROUGHNESS:
Option = Smooth Wall
END
END
END
DOMAIN MODELS:
BUOYANCY MODEL:
Buoyancy Reference Density = 1.28 [kg m^-3]
Gravity X Component = 0 [m s^-2]
Gravity Y Component = -g
Gravity Z Component = 0 [m s^-2]
Option = Buoyant
BUOYANCY REFERENCE LOCATION:
Cartesian Coordinates = 0.0[m],0.0[m],0.0[m]
Option = Cartesian Coordinates
END
END
DOMAIN MOTION:
Option = Stationary
END
MESH DEFORMATION:
Option = None
END
REFERENCE PRESSURE:
Reference Pressure = 98500 [Pa]
END
END
FLUID DEFINITION: Fluid 1
Material = Air Ideal Gas
Option = Material Library
MORPHOLOGY:
Option = Continuous Fluid
END
END
FLUID MODELS:
COMBUSTION MODEL:
Option = None
END
HEAT TRANSFER MODEL:
Include Viscous Work Term = On
Option = Total Energy
END
THERMAL RADIATION MODEL:
Option = None
END
TURBULENCE MODEL:
Option = k epsilon
BUOYANCY TURBULENCE:
Option = None
END
END
TURBULENT WALL FUNCTIONS:
High Speed Model = Off
Option = Scalable
END
END
INITIALISATION:
Option = Automatic
INITIAL CONDITIONS:
Velocity Type = Cartesian
CARTESIAN VELOCITY COMPONENTS:
Option = Automatic with Value
U = 0 [m s^-1]
V = 0 [m s^-1]
W = 0 [m s^-1]
END
STATIC PRESSURE:
Option = Automatic with Value
Relative Pressure = PerfilPresion
END
TEMPERATURE:
Option = Automatic with Value
Temperature = PerfilTemp
END
TURBULENCE INITIAL CONDITIONS:
Option = Medium Intensity and Eddy Viscosity Ratio
END
END
END
POROSITY MODELS:
AREA POROSITY:
Option = Isotropic
END
LOSS MODEL:
Loss Velocity Type = Superficial
Option = Isotropic Loss
ISOTROPIC LOSS MODEL:
Option = Permeability and Loss Coefficient
Permeability = 1E-9 [m^2]
Resistance Loss Coefficient = 0 [m^-1]
END
END
VOLUME POROSITY:
Option = Value
Volume Porosity = 0.7
END
END
SOLID DEFINITION: arboles
Material = Building Board Softwood
Option = Material Library
MORPHOLOGY:
Option = Continuous Solid
END
END
SOLID MODELS:
HEAT TRANSFER MODEL:
Option = None
END
THERMAL RADIATION MODEL:
Option = None
END
END
END
DOMAIN: recinto
Coord Frame = Coord 0
Domain Type = Fluid
Location = recinto
BOUNDARY: Default Fluid Fluid Interface Side 1 1
Boundary Type = INTERFACE
Location = F5281.4,F5282.4
BOUNDARY CONDITIONS:
HEAT TRANSFER:
Option = Conservative Interface Flux
END
MASS AND MOMENTUM:
Option = Conservative Interface Flux
END
TURBULENCE:
Option = Conservative Interface Flux
END
END
END
BOUNDARY: Default Fluid Porous Interface Side 2 1
Boundary Type = INTERFACE

BOUNDARY CONDITIONS:
HEAT TRANSFER:
Option = Conservative Interface Flux
END
MASS AND MOMENTUM:
Option = Conservative Interface Flux
END
TURBULENCE:
Option = Conservative Interface Flux
END
END
END
BOUNDARY: Default Fluid Solid Interface Side 2 1
Boundary Type = INTERFACE

BOUNDARY CONDITIONS:
HEAT TRANSFER:
Option = Adiabatic
END
MASS AND MOMENTUM:
Option = No Slip Wall
END
WALL ROUGHNESS:
Option = Smooth Wall
END
END
END
BOUNDARY: in_viento
Boundary Type = INLET
Location = in_viento
BOUNDARY CONDITIONS:
FLOW REGIME:
Option = Subsonic
END
HEAT TRANSFER:
Option = Static Temperature
Static Temperature = PerfilTemp
END
MASS AND MOMENTUM:
Normal Speed = 1E-4 [m s^-1]
Option = Normal Speed
END
TURBULENCE:
Option = Medium Intensity and Eddy Viscosity Ratio
END
END
END
BOUNDARY: lateral_in
Boundary Type = INLET
Location = lateral_in
BOUNDARY CONDITIONS:
FLOW REGIME:
Option = Subsonic
END
HEAT TRANSFER:
Option = Static Temperature
Static Temperature = PerfilTemp
END
MASS AND MOMENTUM:
Normal Speed = 1E-4 [m s^-1]
Option = Normal Speed
END
TURBULENCE:
Option = Medium Intensity and Eddy Viscosity Ratio
END
END
END
BOUNDARY: lateral_out
Boundary Type = OUTLET
Location = lateral_out
BOUNDARY CONDITIONS:
FLOW REGIME:
Option = Subsonic
END
MASS AND MOMENTUM:
Option = Static Pressure
Relative Pressure = PerfilPresion
END
END
END
BOUNDARY: out_viento
Boundary Type = OUTLET
Location = out_viento
BOUNDARY CONDITIONS:
FLOW REGIME:
Option = Subsonic
END
MASS AND MOMENTUM:
Option = Static Pressure
Relative Pressure = PerfilPresion
END
END
END
BOUNDARY: recinto Default
Boundary Type = WALL
Location = F5280.4
BOUNDARY CONDITIONS:
HEAT TRANSFER:
Option = Adiabatic
END
MASS AND MOMENTUM:
Option = No Slip Wall
END
WALL ROUGHNESS:
Option = Smooth Wall
END
END
END
BOUNDARY: suelo_recinto
Boundary Type = WALL
Location = suelo_recinto
BOUNDARY CONDITIONS:
HEAT TRANSFER:
Fixed Temperature = 269.2 [K]
Option = Fixed Temperature
END
MASS AND MOMENTUM:
Option = No Slip Wall
END
WALL ROUGHNESS:
Option = Smooth Wall
END
END
END
BOUNDARY: techo_recinto
Boundary Type = WALL
Location = techo_recinto
BOUNDARY CONDITIONS:
HEAT TRANSFER:
Fixed Temperature = PerfilTemp
Option = Fixed Temperature
END
MASS AND MOMENTUM:
Option = Free Slip Wall
END
END
END
DOMAIN MODELS:
BUOYANCY MODEL:
Buoyancy Reference Density = 1.28 [kg m^-3]
Gravity X Component = 0 [m s^-2]
Gravity Y Component = -g
Gravity Z Component = 0 [m s^-2]
Option = Buoyant
BUOYANCY REFERENCE LOCATION:
Cartesian Coordinates = 0.0[m],0.0[m],0.0[m]
Option = Cartesian Coordinates
END
END
DOMAIN MOTION:
Option = Stationary
END
MESH DEFORMATION:
Option = None
END
REFERENCE PRESSURE:
Reference Pressure = 98500 [Pa]
END
END
FLUID DEFINITION: Fluid 1
Material = Air Ideal Gas
Option = Material Library
MORPHOLOGY:
Option = Continuous Fluid
END
END
FLUID MODELS:
COMBUSTION MODEL:
Option = None
END
HEAT TRANSFER MODEL:
Include Viscous Work Term = On
Option = Total Energy
END
THERMAL RADIATION MODEL:
Option = None
END
TURBULENCE MODEL:
Option = k epsilon
BUOYANCY TURBULENCE:
Option = None
END
END
TURBULENT WALL FUNCTIONS:
High Speed Model = Off
Option = Scalable
END
END
INITIALISATION:
Option = Automatic
INITIAL CONDITIONS:
Velocity Type = Cartesian
CARTESIAN VELOCITY COMPONENTS:
Option = Automatic with Value
U = 0 [m s^-1]
V = 0 [m s^-1]
W = 0 [m s^-1]
END
STATIC PRESSURE:
Option = Automatic with Value
Relative Pressure = PerfilPresion
END
TEMPERATURE:
Option = Automatic with Value
Temperature = PerfilTemp
END
TURBULENCE INITIAL CONDITIONS:
Option = Medium Intensity and Eddy Viscosity Ratio
END
END
END
END
DOMAIN: rotor
Coord Frame = Coord 0
Domain Type = Fluid
Location = rotor
BOUNDARY: Default Fluid Fluid Interface Side 1
Boundary Type = INTERFACE
Location = F5281.5279,F5282.5279
BOUNDARY CONDITIONS:
HEAT TRANSFER:
Option = Conservative Interface Flux
END
MASS AND MOMENTUM:
Option = Conservative Interface Flux
END
TURBULENCE:
Option = Conservative Interface Flux
END
END
END
BOUNDARY: manto_rotor
Boundary Type = WALL
Frame Type = Rotating
Location = F5280.5279
BOUNDARY CONDITIONS:
HEAT TRANSFER:
Option = Adiabatic
END
MASS AND MOMENTUM:
Option = No Slip Wall
END
WALL ROUGHNESS:
Option = Smooth Wall
END
END
END
DOMAIN MODELS:
BUOYANCY MODEL:
Buoyancy Reference Density = 1.28 [kg m^-3]
Gravity X Component = 0 [m s^-2]
Gravity Y Component = -g
Gravity Z Component = 0 [m s^-2]
Option = Buoyant
BUOYANCY REFERENCE LOCATION:
Cartesian Coordinates = 0.0[m],0.0[m],0.0[m]
Option = Cartesian Coordinates
END
END
DOMAIN MOTION:
Angular Velocity = 0.2 [rev min^-1]
Option = Rotating
AXIS DEFINITION:
Option = Coordinate Axis
Rotation Axis = Coord 1.2
END
END
MESH DEFORMATION:
Option = None
END
REFERENCE PRESSURE:
Reference Pressure = 98500 [Pa]
END
END
FLUID DEFINITION: Fluid 1
Material = Air Ideal Gas
Option = Material Library
MORPHOLOGY:
Option = Continuous Fluid
END
END
FLUID MODELS:
COMBUSTION MODEL:
Option = None
END
HEAT TRANSFER MODEL:
Include Viscous Work Term = On
Option = Total Energy
END
THERMAL RADIATION MODEL:
Option = None
END
TURBULENCE MODEL:
Option = k epsilon
BUOYANCY TURBULENCE:
Option = None
END
END
TURBULENT WALL FUNCTIONS:
High Speed Model = Off
Option = Scalable
END
END
INITIALISATION:
Frame Type = Stationary
Option = Automatic
INITIAL CONDITIONS:
Velocity Type = Cartesian
CARTESIAN VELOCITY COMPONENTS:
Option = Automatic with Value
U = 0 [m s^-1]
V = 0 [m s^-1]
W = 0 [m s^-1]
END
STATIC PRESSURE:
Option = Automatic with Value
Relative Pressure = PerfilPresion
END
TEMPERATURE:
Option = Automatic with Value
Temperature = PerfilTemp
END
TURBULENCE INITIAL CONDITIONS:
Option = Medium Intensity and Eddy Viscosity Ratio
END
END
END
SUBDOMAIN: mom source
Coord Frame = Coord 0
Location = rotor
SOURCES:
MOMENTUM SOURCE:
GENERAL MOMENTUM SOURCE:
Include Coefficient in Rhie Chow = On
Momentum Source Coefficient = -5E2 [kg m^-3 s^-1]
Momentum Source X Component = -5E2[kg m^-3 s^-1]*((Velocity u)- \
20*cos(pi/180*7)*sin(phi) [m s^-1])
Momentum Source Y Component = -5E2[kg m^-3 s^-1]*((Velocity \
v)+20*sin(pi/180*7) [m s^-1])
Momentum Source Z Component = -5E2[kg m^-3 s^-1]*((Velocity w)- \
20*cos(pi/180*7)*cos(phi) [m s^-1])
Option = Cartesian Components
Redistribute in Rhie Chow = On
END
END
END
END
END
DOMAIN INTERFACE: Default Fluid Fluid Interface
Boundary List1 = Default Fluid Fluid Interface Side 1 1
Boundary List2 = Default Fluid Fluid Interface Side 1
Interface Type = Fluid Fluid
INTERFACE MODELS:
Option = General Connection
FRAME CHANGE:
Option = Frozen Rotor
END
MASS AND MOMENTUM:
Option = Conservative Interface Flux
MOMENTUM INTERFACE MODEL:
Option = None
END
END
PITCH CHANGE:
Option = Specified Pitch Angles
Pitch Angle Side1 = 360 [degree]
Pitch Angle Side2 = 360 [degree]
END
END
MESH CONNECTION:
Option = GGI
END
END
DOMAIN INTERFACE: Default Fluid Porous Interface
Boundary List1 = Default Fluid Porous Interface Side 1 1
Boundary List2 = Default Fluid Porous Interface Side 2 1
Interface Type = Fluid Porous
INTERFACE MODELS:
Option = General Connection
FRAME CHANGE:
Option = None
END
MASS AND MOMENTUM:
Option = Conservative Interface Flux
MOMENTUM INTERFACE MODEL:
Option = None
END
END
PITCH CHANGE:
Option = None
END
END
MESH CONNECTION:
Option = GGI
END
END
DOMAIN INTERFACE: Default Fluid Solid Interface
Boundary List1 = Default Fluid Solid Interface Side 1 1
Boundary List2 = Default Fluid Solid Interface Side 2 1
Interface Type = Fluid Solid
INTERFACE MODELS:
Option = General Connection
FRAME CHANGE:
Option = Frozen Rotor
END
PITCH CHANGE:
Option = Specified Pitch Angles
Pitch Angle Side1 = 360 [degree]
Pitch Angle Side2 = 360 [degree]
END
END

Here is the last pic.

here is it sorry lol

I think the problem will be worst once you do a grid sensitivity analysis that will force you to reduce the time step to remain the computation stable.
Why don't you use an implicit approach?

What do you mean by implicit approach exactly?

I have more than 4 years without using CFX, but if I am not mistaken you have different implicit schemes, which are not very accurate, but still are very good for good results.
Try to use a high resolution scheme, that changes between first order and second order Euler.

I see lots of issues.
* You have viscous work on. Unless you intend to model viscous heating turn it off. I can't see how viscous heating is significant here.

* Why are you modelling the solid? This makes this a CHT simulation which is much more complex. I cannot see why you need to model the solid.

* You have modelled the blower as a rotating domain. It would be MUCH simpler to have one stationary domain for the whole simulation and model the blower as a rotating momentum source. By this I just mean the X,Y and Z components of the momentum source are varied as a function of time to make it a rotating blower.

* You have the total energy option selected. Why do you need that? A thermal energy model will be much simpler and robust and I suspect will have enough physics for this case.

* You have the frame change model as frozen rotor. If you want to model the rotation of the blower then shouldn't that be Transient Rotor Stator?

* What is the purpose of the porous model? This is yet another model which will add complexity.

Julio: CFX is a fully implicit solver (at least with these physics models it is). There are no options available to make it otherwise.