|
[Sponsors] |
November 5, 2017, 21:14 |
Question about adaptive timestepping
|
#1 |
Member
Join Date: Oct 2017
Posts: 89
Rep Power: 9 |
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. |
|
November 6, 2017, 01:12 |
|
#2 |
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,830
Rep Power: 144 |
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. |
|
November 6, 2017, 15:38 |
|
#3 |
Senior Member
Erik
Join Date: Feb 2011
Location: Earth (Land portion)
Posts: 1,184
Rep Power: 23 |
Also, besides mesh quality, mesh size makes a large difference as well. you can use a larger time step with a larger mesh.
|
|
November 6, 2017, 19:32 |
|
#4 |
Member
Join Date: Oct 2017
Posts: 89
Rep Power: 9 |
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 |
|
November 6, 2017, 19:40 |
|
#5 |
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,830
Rep Power: 144 |
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. |
|
November 6, 2017, 19:50 |
|
#6 |
Member
Join Date: Oct 2017
Posts: 89
Rep Power: 9 |
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 |
|
November 6, 2017, 21:17 |
|
#7 |
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,830
Rep Power: 144 |
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 |
|
November 8, 2017, 11:16 |
|
#8 |
Member
Join Date: Oct 2017
Posts: 89
Rep Power: 9 |
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 :/ |
|
November 8, 2017, 17:39 |
|
#9 |
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,830
Rep Power: 144 |
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? |
|
November 9, 2017, 00:42 |
|
#10 |
Member
Join Date: Oct 2017
Posts: 89
Rep Power: 9 |
It runs fine judging by my monitors but my huge problem is the tiny timestep size due to adaptive timestepping
|
|
November 9, 2017, 00:50 |
|
#11 |
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,830
Rep Power: 144 |
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? |
|
November 9, 2017, 14:24 |
|
#12 |
Member
Join Date: Oct 2017
Posts: 89
Rep Power: 9 |
how can i post my CCL?
|
|
November 9, 2017, 16:08 |
|
#13 |
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,830
Rep Power: 144 |
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.
|
|
November 9, 2017, 17:34 |
|
#14 |
Member
Join Date: Oct 2017
Posts: 89
Rep Power: 9 |
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 |
|
November 9, 2017, 17:37 |
|
#15 |
Member
Join Date: Oct 2017
Posts: 89
Rep Power: 9 |
Here is the last pic.
|
|
November 9, 2017, 17:42 |
|
#16 |
Member
Join Date: Oct 2017
Posts: 89
Rep Power: 9 |
here is it sorry lol
|
|
November 9, 2017, 18:37 |
|
#17 |
Senior Member
|
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? |
|
November 9, 2017, 18:39 |
|
#18 |
Member
Join Date: Oct 2017
Posts: 89
Rep Power: 9 |
||
November 9, 2017, 18:53 |
|
#19 |
Senior Member
|
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. |
|
November 9, 2017, 21:16 |
|
#20 |
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,830
Rep Power: 144 |
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. |
|
Thread Tools | Search this Thread |
Display Modes | |
|
|
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 |