[kalm]

hello everyone. I am trying to analyze an tested centrifugal fan with cfx. CFX results are 20% lower than the test results at high pressures and close to the test results at low pressures. I tried all input and output combinations but the results did not change. I ran it with transient and the results are still incorrect. When I looked at the flow with the cfd post, I noticed that there was a reverse flow in front of the wing. Where do you think the problem might be? The photo about this is attached.

[ghorrocks]

A large separation like that means the design is not running very well and will have large losses. This is a real effect, and is the reason turbomachines have a peak performance point, as off the design point things like this will happen.

So if the expected performance is significantly higher than CFX predicts, and CFX predicts a large separation like that (which would cause a large loss in performance) then the question is who did CFX incorrectly predict a large separation. It could be:
* Inappropriate physical model (eg wrong turbulence model) - what turbulence model did you use?
* Inaccurate simulation technique - did you do a mesh sensitivity study and a convergence sensitivity study? See https://www.cfd-online.com/Wiki/Ansy..._inaccurate.3F
* Boundary conditions not specified correctly - are you sure your boundary conditions match what the experiment did? Things like surface roughness, upstream turbulence are key factors as well.
* Poor experimental accuracy

[kalm]

thank you for the answer . I tried SST and k-epsilon turbulence model, the result is the same. I also did a mesh density study. There is no convergence problem, even very fast convergence. I analyzed only the propeller without an interface with the mesh I created in Turbogrid. The vector lines appear smooth at the total pressure inlet and mass outlet. The mass inlet is at the static pressure outlet and when I interface it to the outlet of the propeller, the vector lines are wrong again.

[ghorrocks]

I tried SST and k-epsilon turbulence model, the result is the same.

There are many short comings common to k-e and SST. You might need to go beyond those models.

I also did a mesh density study.

What meshes did you look at?

Can you show the experimental results you are comparing against, and the results you are getting? ALso please attach your output file.

[Opaque]

Originally Posted by kalm

hello everyone. I am trying to analyze an tested centrifugal fan with cfx. CFX results are 20% lower than the test results at high pressures and close to the test results at low pressures. I tried all input and output combinations but the results did not change. I ran it with transient and the results are still incorrect. When I looked at the flow with the cfd post, I noticed that there was a reverse flow in front of the wing. Where do you think the problem might be? The photo about this is attached.

Are you running a full model?
How many elements per passage of the wheel are you using?
What is the mesh density near the walls? Y+ near 1?

[kalm]

Experimental results: 3500 Pa pressure at 2.96 m3/s flow rate, 2950 Pa at the stage interface, 2650 Pa at the frozen interface in the analysis. Even if I increase the number of meshes, the results do not change much. Mesh photos are attached.
LIBRARY:
CEL:
EXPRESSIONS:
fan pst = massFlowAve(Pressure )@S1 Outlet-massFlowAve(Pressure )@S1 \
Inlet
END
END
MATERIAL: Air Ideal Gas
Material Description = Air Ideal Gas (constant Cp)
Material Group = Air Data, Calorically Perfect Ideal Gases
Option = Pure Substance
Thermodynamic State = Gas
PROPERTIES:
Option = General Material
EQUATION OF STATE:
Molar Mass = 28.96 [kg kmol^-1]
Option = Ideal Gas
END
SPECIFIC HEAT CAPACITY:
Option = Value
Specific Heat Capacity = 1.0044E+03 [J kg^-1 K^-1]
Specific Heat Type = Constant Pressure
END
REFERENCE STATE:
Option = Specified Point
Reference Pressure = 1 [atm]
Reference Specific Enthalpy = 0. [J/kg]
Reference Specific Entropy = 0. [J/kg/K]
Reference Temperature = 25 [C]
END
DYNAMIC VISCOSITY:
Dynamic Viscosity = 1.831E-05 [kg m^-1 s^-1]
Option = Value
END
THERMAL CONDUCTIVITY:
Option = Value
Thermal Conductivity = 2.61E-2 [W m^-1 K^-1]
END
ABSORPTION COEFFICIENT:
Absorption Coefficient = 0.01 [m^-1]
Option = Value
END
SCATTERING COEFFICIENT:
Option = Value
Scattering Coefficient = 0.0 [m^-1]
END
REFRACTIVE INDEX:
Option = Value
Refractive Index = 1.0 [m m^-1]
END
END
END
MATERIAL: Air at 25 C
Material Description = Air at 25 C and 1 atm (dry)
Material Group = Air Data, Constant Property Gases
Option = Pure Substance
Thermodynamic State = Gas
PROPERTIES:
Option = General Material
EQUATION OF STATE:
Density = 1.185 [kg m^-3]
Molar Mass = 28.96 [kg kmol^-1]
Option = Value
END
SPECIFIC HEAT CAPACITY:
Option = Value
Specific Heat Capacity = 1.0044E+03 [J kg^-1 K^-1]
Specific Heat Type = Constant Pressure
END
REFERENCE STATE:
Option = Specified Point
Reference Pressure = 1 [atm]
Reference Specific Enthalpy = 0. [J/kg]
Reference Specific Entropy = 0. [J/kg/K]
Reference Temperature = 25 [C]
END
DYNAMIC VISCOSITY:
Dynamic Viscosity = 1.831E-05 [kg m^-1 s^-1]
Option = Value
END
THERMAL CONDUCTIVITY:
Option = Value
Thermal Conductivity = 2.61E-02 [W m^-1 K^-1]
END
ABSORPTION COEFFICIENT:
Absorption Coefficient = 0.01 [m^-1]
Option = Value
END
SCATTERING COEFFICIENT:
Option = Value
Scattering Coefficient = 0.0 [m^-1]
END
REFRACTIVE INDEX:
Option = Value
Refractive Index = 1.0 [m m^-1]
END
THERMAL EXPANSIVITY:
Option = Value
Thermal Expansivity = 0.003356 [K^-1]
END
END
END
MATERIAL: Aluminium
Material Group = CHT Solids, Particle Solids
Option = Pure Substance
Thermodynamic State = Solid
PROPERTIES:
Option = General Material
EQUATION OF STATE:
Density = 2702 [kg m^-3]
Molar Mass = 26.98 [kg kmol^-1]
Option = Value
END
SPECIFIC HEAT CAPACITY:
Option = Value
Specific Heat Capacity = 9.03E+02 [J kg^-1 K^-1]
END
REFERENCE STATE:
Option = Specified Point
Reference Specific Enthalpy = 0 [J/kg]
Reference Specific Entropy = 0 [J/kg/K]
Reference Temperature = 25 [C]
END
THERMAL CONDUCTIVITY:
Option = Value
Thermal Conductivity = 237 [W m^-1 K^-1]
END
END
END
MATERIAL: Copper
Material Group = CHT Solids, Particle Solids
Option = Pure Substance
Thermodynamic State = Solid
PROPERTIES:
Option = General Material
EQUATION OF STATE:
Density = 8933 [kg m^-3]
Molar Mass = 63.55 [kg kmol^-1]
Option = Value
END
SPECIFIC HEAT CAPACITY:
Option = Value
Specific Heat Capacity = 3.85E+02 [J kg^-1 K^-1]
END
REFERENCE STATE:
Option = Specified Point
Reference Specific Enthalpy = 0 [J/kg]
Reference Specific Entropy = 0 [J/kg/K]
Reference Temperature = 25 [C]
END
THERMAL CONDUCTIVITY:
Option = Value
Thermal Conductivity = 401.0 [W m^-1 K^-1]
END
END
END
MATERIAL: Soot
Material Group = Soot
Option = Pure Substance
Thermodynamic State = Solid
PROPERTIES:
Option = General Material
EQUATION OF STATE:
Density = 2000 [kg m^-3]
Molar Mass = 12 [kg kmol^-1]
Option = Value
END
REFERENCE STATE:
Option = Automatic
END
ABSORPTION COEFFICIENT:
Absorption Coefficient = 0 [m^-1]
Option = Value
END
END
END
MATERIAL: Steel
Material Group = CHT Solids, Particle Solids
Option = Pure Substance
Thermodynamic State = Solid
PROPERTIES:
Option = General Material
EQUATION OF STATE:
Density = 7854 [kg m^-3]
Molar Mass = 55.85 [kg kmol^-1]
Option = Value
END
SPECIFIC HEAT CAPACITY:
Option = Value
Specific Heat Capacity = 4.34E+02 [J kg^-1 K^-1]
END
REFERENCE STATE:
Option = Specified Point
Reference Specific Enthalpy = 0 [J/kg]
Reference Specific Entropy = 0 [J/kg/K]
Reference Temperature = 25 [C]
END
THERMAL CONDUCTIVITY:
Option = Value
Thermal Conductivity = 60.5 [W m^-1 K^-1]
END
END
END
MATERIAL: Water
Material Description = Water (liquid)
Material Group = Water Data, Constant Property Liquids
Option = Pure Substance
Thermodynamic State = Liquid
PROPERTIES:
Option = General Material
EQUATION OF STATE:
Density = 997.0 [kg m^-3]
Molar Mass = 18.02 [kg kmol^-1]
Option = Value
END
SPECIFIC HEAT CAPACITY:
Option = Value
Specific Heat Capacity = 4181.7 [J kg^-1 K^-1]
Specific Heat Type = Constant Pressure
END
REFERENCE STATE:
Option = Specified Point
Reference Pressure = 1 [atm]
Reference Specific Enthalpy = 0.0 [J/kg]
Reference Specific Entropy = 0.0 [J/kg/K]
Reference Temperature = 25 [C]
END
DYNAMIC VISCOSITY:
Dynamic Viscosity = 8.899E-4 [kg m^-1 s^-1]
Option = Value
END
THERMAL CONDUCTIVITY:
Option = Value
Thermal Conductivity = 0.6069 [W m^-1 K^-1]
END
ABSORPTION COEFFICIENT:
Absorption Coefficient = 1.0 [m^-1]
Option = Value
END
SCATTERING COEFFICIENT:
Option = Value
Scattering Coefficient = 0.0 [m^-1]
END
REFRACTIVE INDEX:
Option = Value
Refractive Index = 1.0 [m m^-1]
END
THERMAL EXPANSIVITY:
Option = Value
Thermal Expansivity = 2.57E-04 [K^-1]
END
END
END
MATERIAL: Water Ideal Gas
Material Description = Water Vapour Ideal Gas (100 C and 1 atm)
Material Group = Calorically Perfect Ideal Gases, Water Data
Option = Pure Substance
Thermodynamic State = Gas
PROPERTIES:
Option = General Material
EQUATION OF STATE:
Molar Mass = 18.02 [kg kmol^-1]
Option = Ideal Gas
END
SPECIFIC HEAT CAPACITY:
Option = Value
Specific Heat Capacity = 2080.1 [J kg^-1 K^-1]
Specific Heat Type = Constant Pressure
END
REFERENCE STATE:
Option = Specified Point
Reference Pressure = 1.014 [bar]
Reference Specific Enthalpy = 0. [J/kg]
Reference Specific Entropy = 0. [J/kg/K]
Reference Temperature = 100 [C]
END
DYNAMIC VISCOSITY:
Dynamic Viscosity = 9.4E-06 [kg m^-1 s^-1]
Option = Value
END
THERMAL CONDUCTIVITY:
Option = Value
Thermal Conductivity = 193E-04 [W m^-1 K^-1]
END
ABSORPTION COEFFICIENT:
Absorption Coefficient = 1.0 [m^-1]
Option = Value
END
SCATTERING COEFFICIENT:
Option = Value
Scattering Coefficient = 0.0 [m^-1]
END
REFRACTIVE INDEX:
Option = Value
Refractive Index = 1.0 [m m^-1]
END
END
END
END
FLOW: steady
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 = Steady State
EXTERNAL SOLVER COUPLING:
Option = None
END
END
DOMAIN: R1
Coord Frame = Coord 0
Domain Type = Fluid
Location = impeller
BOUNDARY: Domain Interface 1 Side 1
Boundary Type = INTERFACE
Location = inflow impeller
BOUNDARY CONDITIONS:
MASS AND MOMENTUM:
Option = Conservative Interface Flux
END
TURBULENCE:
Option = Conservative Interface Flux
END
END
END
BOUNDARY: Domain Interface 2 Side 1
Boundary Type = INTERFACE
Location = outflow impeller
BOUNDARY CONDITIONS:
MASS AND MOMENTUM:
Option = Conservative Interface Flux
END
TURBULENCE:
Option = Conservative Interface Flux
END
END
END
BOUNDARY: R1 Blade
Boundary Type = WALL
Coord Frame = Coord 0
Frame Type = Rotating
Location = blade
BOUNDARY CONDITIONS:
MASS AND MOMENTUM:
Option = No Slip Wall
END
WALL ROUGHNESS:
Option = Smooth Wall
END
END
END
BOUNDARY: R1 Hub
Boundary Type = WALL
Coord Frame = Coord 0
Frame Type = Rotating
Location = hub
BOUNDARY CONDITIONS:
MASS AND MOMENTUM:
Option = No Slip Wall
END
WALL ROUGHNESS:
Option = Smooth Wall
END
END
END
BOUNDARY: R1 Shroud
Boundary Type = WALL
Coord Frame = Coord 0
Frame Type = Rotating
Location = shroud
BOUNDARY CONDITIONS:
MASS AND MOMENTUM:
Option = No Slip Wall
END
WALL ROUGHNESS:
Option = Smooth Wall
END
END
END
DOMAIN MODELS:
BUOYANCY MODEL:
Option = Non Buoyant
END
DOMAIN MOTION:
Alternate Rotation Model = true
Angular Velocity = 2950 [rev min^-1]
Option = Rotating
AXIS DEFINITION:
Option = Coordinate Axis
Rotation Axis = Coord 0.3
END
END
MESH DEFORMATION:
Option = None
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 = SST
REATTACHMENT MODIFICATION:
Option = Reattachment Production
END
TRANSITIONAL TURBULENCE:
Option = Fully Turbulent
END
END
TURBULENT WALL FUNCTIONS:
Option = Automatic
END
END
INITIALISATION:
Coord Frame = Coord 0
Frame Type = Rotating
Option = Automatic
INITIAL CONDITIONS:
Velocity Type = Cartesian
CARTESIAN VELOCITY COMPONENTS:
Option = Automatic
END
STATIC PRESSURE:
Option = Automatic
END
TURBULENCE INITIAL CONDITIONS:
Option = Medium Intensity and Eddy Viscosity Ratio
END
END
END
END
DOMAIN: S1
Coord Frame = Coord 0
Domain Type = Fluid
Location = volute
BOUNDARY: Domain Interface 1 Side 2
Boundary Type = INTERFACE
Location = impeller volute in
BOUNDARY CONDITIONS:
MASS AND MOMENTUM:
Option = Conservative Interface Flux
END
TURBULENCE:
Option = Conservative Interface Flux
END
END
END
BOUNDARY: Domain Interface 2 Side 2
Boundary Type = INTERFACE
Location = impeller volute out
BOUNDARY CONDITIONS:
MASS AND MOMENTUM:
Option = Conservative Interface Flux
END
TURBULENCE:
Option = Conservative Interface Flux
END
END
END
BOUNDARY: S1 Default
Boundary Type = WALL
Location = \
F268.288,F269.288,F270.288,F271.288,F272.288,F273. 288,F274.288,F275.28\
8,F276.288,F277.288,F278.288,F279.288,F280.288,F28 1.288,F283.288,F284.\
288,F285.288,F286.288,F291.288,F292.288,F293.288,F 294.288,F295.288,F29\
6.288,F297.288,F298.288
BOUNDARY CONDITIONS:
MASS AND MOMENTUM:
Option = No Slip Wall
END
WALL ROUGHNESS:
Option = Smooth Wall
END
END
END
BOUNDARY: S1 Inlet
Boundary Type = INLET
Coord Frame = Coord 0
Location = inlet
BOUNDARY CONDITIONS:
FLOW DIRECTION:
Option = Normal to Boundary Condition
END
FLOW REGIME:
Option = Subsonic
END
MASS AND MOMENTUM:
Option = Total Pressure
Relative Pressure = 0 [atm]
END
TURBULENCE:
Option = Medium Intensity and Eddy Viscosity Ratio
END
END
END
BOUNDARY: S1 Outlet
Boundary Type = OUTLET
Location = outlet
BOUNDARY CONDITIONS:
FLOW REGIME:
Option = Subsonic
END
MASS AND MOMENTUM:
Mass Flow Rate = 3.52 [kg s^-1]
Mass Flow Rate Area = As Specified
Option = Mass Flow Rate
END
END
END
DOMAIN MODELS:
BUOYANCY MODEL:
Option = Non Buoyant
END
DOMAIN MOTION:
Option = Stationary
END
MESH DEFORMATION:
Option = None
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 = SST
REATTACHMENT MODIFICATION:
Option = Reattachment Production
END
TRANSITIONAL TURBULENCE:
Option = Fully Turbulent
END
END
TURBULENT WALL FUNCTIONS:
Option = Automatic
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 = General Connection
FRAME CHANGE:
Option = Stage
DOWNSTREAM VELOCITY CONSTRAINT:
Frame Type = Rotating
Option = Constant Total Pressure
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: Domain Interface 2
Boundary List1 = Domain Interface 2 Side 1
Boundary List2 = Domain Interface 2 Side 2
Interface Type = Fluid Fluid
INTERFACE MODELS:
Option = General Connection
FRAME CHANGE:
Option = Stage
DOWNSTREAM VELOCITY CONSTRAINT:
Frame Type = Rotating
Option = Constant Total Pressure
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
OUTPUT CONTROL:
MONITOR OBJECTS:
MONITOR BALANCES:
Option = Full
END
MONITOR FORCES:
Option = Full
END
MONITOR PARTICLES:
Option = Full
END
MONITOR POINT: pst
Coord Frame = Coord 0
Expression Value = fan pst
Option = Expression
END
MONITOR RESIDUALS:
Option = Full
END
MONITOR TOTALS:
Option = Full
END
END
RESULTS:
File Compression Level = Default
Option = Standard
END
END
SOLVER CONTROL:
Turbulence Numerics = High Resolution
ADVECTION SCHEME:
Option = High Resolution
END
CONVERGENCE CONTROL:
Maximum Number of Iterations = 200
Minimum Number of Iterations = 1
Physical Timescale = 0.01 [s]
Timescale Control = Physical Timescale
END
CONVERGENCE CRITERIA:
Residual Target = 1e-5
Residual Type = RMS
END
DYNAMIC MODEL CONTROL:
Global Dynamic Model Control = Yes
END
INTERRUPT CONTROL:
Option = Any Interrupt
CONVERGENCE CONDITIONS:
Option = Default Conditions
END
END
END
END

[kalm]

Originally Posted by Opaque

Are you running a full model?
How many elements per passage of the wheel are you using?
What is the mesh density near the walls? Y+ near 1?

I also tried with the full model and single passage. I made 12 blades with a single blade and 1M mesh, but the results still do not change. Max y+ 62 in the whole model.

[kalm]

Originally Posted by ghorrocks

There are many short comings common to k-e and SST. You might need to go beyond those models.



What meshes did you look at?

Can you show the experimental results you are comparing against, and the results you are getting? ALso please attach your output file.

Hello . I noticed something like this. As the blade height decreases, the pressure should decrease. In my analysis, by decreasing the blade height from 100 mm to 90 mm, the pressure increases. While the blade height is 100mm, the pressure is 2950 Pa, while the blade height is 90mm, the pressure is 3280 Pa.

[Opaque]

If your mesh has a Y+ on the boundary of 62, there is absolutely no point in using SST. SST requires Y+ <= 1 throughout all the walls.

If your full model is not capturing the experimental data, then you have a bigger problem:

1 - Either the experimental data is bogus
2 - The setup is incorrect somewhere, for example:
a - it may not be representative of the experiment.
b - your transient is not timestep independent
c - your mesh refinement is not capturing the regions of high gradients
d - your frame change interface may be incorrectly set
e - have you checked the impeller is rotating in the correct direction? I have seen it all in rotor-stator setups
f - may I ask why are you running transition at all? Keep it simple: no transition, no reattachment
g - why are you not using Automatic for the Pitch Change model?
h - Finally, you got to be kidding using an incompressible material in a compressor/fan. You MUST use Air Ideal Gas. Air at 25C is incompressible

[kalm]

Which turbulence model do you recommend? In this way, the results of a different fan that I analyzed completely matched the experimental results and there was no reverse flow around the blade. I think the reverse flow around the blade of this fan causes the results to be incorrect.

[Gert-Jan]

- In these cases not solely look to Velocity but also at Velocity at Stationary Frame.

- Your vectors are very unclear. Please add better pictures where direction is more clear. (e.g, white background, equally spaced vectors, uniform length, projected etc.)

- Like Opaque mentioned, check the rotation direction. In >95% of my setups, the rotation direction has to be negative to let it rotate in the required direction.

- Having these recirculations has nothing to do with right or wrong. These could be realistic very well, depending on the operational point. Can you explain where on the curve you are operating?

- I would start with Frozen rotor and Automatic Pitch. Since it is 360°, CFX will be able to determine the best settings automatically.

- Turn off the Alternate Rotation model. Mostly not required.

- Start with Auto timescale. I think a physical timestep of 0.01[s] is way too large. With almost 3000 rpm, i.e. 50Hz, it takes 0.02[s] to make one revolution.

- Alternatively go to transient. I have seen bad results turn to good ones, by switching to transient. Especially with radial fans.

- Don't use Transition at this stage. Only use it as a very, very, very last resort. Just use SST. Should be fine. As long as Y+ is below 300, I would not expect a major difference.

[kalm]

Thank you very much for your answer. I will try your advice. I work at the most productive point of the curve. Vector, convergence and static pressure screen photos are attached.

[ghorrocks]

Your blade geometry is just a simple curved plate. I would expect that to separate at just about every flow condition (including peak performance). In fact I would think it very difficult to find a condition where that geometry would not separate.

For the flow to be attached you need carefully shaped blades with airfoil cross-sections. It would need carefully angled entry and exit angles.

In other words - I think your CFX results are correct, this design should have a big separation in it.

[kalm]

Thank you very much for your reply . You are so right Glenn. I had previously analyzed a fan with a different geometry with a lower time interval, its results matched the experimental results, there was also separation in the blades of that fan. Now I will try this fan with a low time step.
CFD Online is a very nice site. You are doing great work by taking the time to help. Thank you very much again. Kind regards .

[kalm]

Hello friends . I ran the fan test again and the results were the same as the previous experiment. I confirmed that my analysis results were incorrect. If I start the analysis with automatic time scale, it matches the experimental results, but the residuals do not go below 1^10-4. When I increase the automatic time scale factor in the solver, the pressure drops rapidly. Where could the problem be? I would be very happy if you help.

[Opaque]

Originally Posted by kalm

Hello friends . I ran the fan test again and the results were the same as the previous experiment. I confirmed that my analysis results were incorrect. If I start the analysis with automatic time scale, it matches the experimental results, but the residuals do not go below 1^10-4. When I increase the automatic time scale factor in the solver, the pressure drops rapidly. Where could the problem be? I would be very happy if you help.

The solution should be independent of the Timescale you use. The timescale only changes how fast the solution converges or diverges, nothing else.

When you increase your timescale, what happens to the residuals? Up/down, stays fixed?

When the residuals stay at a fixed value above expectations (mine expectation is 1E-5 or below), you should go to
Output Control/Results/Output Equation Residuals = All

Run the simulation, post-process the results (converged or not) and check where the region of large residuals are. Try to understand what is happening around there: mesh quality, unphysical results, stagnant flow, etc.

[kalm]

Thank you for your reply. When I increase the time scale, the residuals quickly decrease to 1e-5 and the pressure quickly moves away from the experimental results. When I switch from steady to transient with adaptive time step, the residuals drop below 1e-5 in the first few iterations. In CFD post, residues remain high in regions where the speed is low. Network quality seems good in these regions. Do you have any other suggestions regarding this?

[ghorrocks]

Can you show an image where you show the high residual regions?

When you run transient you will need to run for enough time steps to capture any transient behaviour. This means a few cycles of any transient behaviour. You cannot just run a time step or two.

[kalm]

Thank you for your answer . I ran a new analysis to view the residuals. photos have been added. I tried everything you said but I couldn't find where I was doing wrong. Do you have any other suggestions? Thank you very much

[ghorrocks]

You will need to redo the residuals images with a higher residual. The setting you currently have is showing too much. You need to look at the worst bit where you are only starting to get a small bubble of volume as that will show where the most difficult locations are.