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

Question about adaptive timestepping

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

Like Tree2Likes

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   November 5, 2017, 21:14
Default Question about adaptive timestepping
  #1
Member
 
Join Date: Oct 2017
Posts: 89
Rep Power: 3
Guille1811 is on a distinguished road
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.
Guille1811 is offline   Reply With Quote

Old   November 6, 2017, 01:12
Default
  #2
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 15,628
Rep Power: 120
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
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.
ghorrocks is offline   Reply With Quote

Old   November 6, 2017, 15:38
Default
  #3
Senior Member
 
Erik
Join Date: Feb 2011
Location: Earth (Land portion)
Posts: 837
Rep Power: 16
evcelica is on a distinguished road
Also, besides mesh quality, mesh size makes a large difference as well. you can use a larger time step with a larger mesh.
evcelica is offline   Reply With Quote

Old   November 6, 2017, 19:32
Default
  #4
Member
 
Join Date: Oct 2017
Posts: 89
Rep Power: 3
Guille1811 is on a distinguished road
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
Guille1811 is offline   Reply With Quote

Old   November 6, 2017, 19:40
Default
  #5
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 15,628
Rep Power: 120
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
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.
ghorrocks is offline   Reply With Quote

Old   November 6, 2017, 19:50
Default
  #6
Member
 
Join Date: Oct 2017
Posts: 89
Rep Power: 3
Guille1811 is on a distinguished road
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
Guille1811 is offline   Reply With Quote

Old   November 6, 2017, 21:17
Default
  #7
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 15,628
Rep Power: 120
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
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
ghorrocks is offline   Reply With Quote

Old   November 8, 2017, 11:16
Default
  #8
Member
 
Join Date: Oct 2017
Posts: 89
Rep Power: 3
Guille1811 is on a distinguished road
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 :/
Guille1811 is offline   Reply With Quote

Old   November 8, 2017, 17:39
Default
  #9
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 15,628
Rep Power: 120
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
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?
ghorrocks is offline   Reply With Quote

Old   November 9, 2017, 00:42
Default
  #10
Member
 
Join Date: Oct 2017
Posts: 89
Rep Power: 3
Guille1811 is on a distinguished road
It runs fine judging by my monitors but my huge problem is the tiny timestep size due to adaptive timestepping
Guille1811 is offline   Reply With Quote

Old   November 9, 2017, 00:50
Default
  #11
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 15,628
Rep Power: 120
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
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?
ghorrocks is offline   Reply With Quote

Old   November 9, 2017, 14:24
Default
  #12
Member
 
Join Date: Oct 2017
Posts: 89
Rep Power: 3
Guille1811 is on a distinguished road
how can i post my CCL?
Guille1811 is offline   Reply With Quote

Old   November 9, 2017, 16:08
Default
  #13
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 15,628
Rep Power: 120
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
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.
ghorrocks is offline   Reply With Quote

Old   November 9, 2017, 17:34
Default
  #14
Member
 
Join Date: Oct 2017
Posts: 89
Rep Power: 3
Guille1811 is on a distinguished road
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
Attached Images
File Type: png isometric view.PNG (14.0 KB, 6 views)
File Type: png side view.PNG (5.3 KB, 4 views)
File Type: png closeup side view cilinder and motor.PNG (4.0 KB, 3 views)
File Type: png upper view (note the position of the cilinder - engine).PNG (17.1 KB, 3 views)
File Type: png isometric view section plane meshing.PNG (28.1 KB, 6 views)
Guille1811 is offline   Reply With Quote

Old   November 9, 2017, 17:37
Default
  #15
Member
 
Join Date: Oct 2017
Posts: 89
Rep Power: 3
Guille1811 is on a distinguished road
Here is the last pic.
Guille1811 is offline   Reply With Quote

Old   November 9, 2017, 17:42
Default
  #16
Member
 
Join Date: Oct 2017
Posts: 89
Rep Power: 3
Guille1811 is on a distinguished road
here is it sorry lol
Attached Images
File Type: png side view meshing.PNG (94.3 KB, 10 views)
Guille1811 is offline   Reply With Quote

Old   November 9, 2017, 18:37
Default
  #17
Senior Member
 
Julio Mendez
Join Date: Apr 2009
Location: Fairburn, GA. USA
Posts: 278
Rep Power: 13
juliom is on a distinguished road
Send a message via Skype™ to juliom
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?
juliom is offline   Reply With Quote

Old   November 9, 2017, 18:39
Default
  #18
Member
 
Join Date: Oct 2017
Posts: 89
Rep Power: 3
Guille1811 is on a distinguished road
Quote:
Originally Posted by juliom View Post
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?
Guille1811 is offline   Reply With Quote

Old   November 9, 2017, 18:53
Default
  #19
Senior Member
 
Julio Mendez
Join Date: Apr 2009
Location: Fairburn, GA. USA
Posts: 278
Rep Power: 13
juliom is on a distinguished road
Send a message via Skype™ to juliom
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.
juliom is offline   Reply With Quote

Old   November 9, 2017, 21:16
Default
  #20
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 15,628
Rep Power: 120
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
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.
juliom and ZeroState like this.
ghorrocks is offline   Reply With Quote

Reply

Thread Tools Search this Thread
Search this Thread:

Advanced Search
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
Aitken adaptive under-relaxation for FSI WiWo OpenFOAM 5 January 4, 2016 01:49
Question Re Engineering Data Source imnull ANSYS 0 March 5, 2012 13:51
internal field question - PitzDaily Case atareen64 OpenFOAM Running, Solving & CFD 2 January 26, 2011 15:26
A question on adaptive remeshing or mesh deformation for handling object motions daveatstyacht OpenFOAM 10 November 13, 2010 09:29
Poisson Solver question Suresh Main CFD Forum 3 August 12, 2005 04:37


All times are GMT -4. The time now is 18:47.