|
[Sponsors] |
Set Density with presssure,the result is not correct |
|
LinkBack | Thread Tools | Search this Thread | Display Modes |
May 2, 2024, 11:39 |
Set Density with presssure,the result is not correct
|
#1 |
New Member
Join Date: Jan 2022
Posts: 20
Rep Power: 4 |
Hi Everyone,
I am trying to simulate an incompressible fluid flow in a pump turbine. I wanted to study the effect of micro-compression of water on hydraulic machinery. I added the density change with pressure through the CEL expression, without considering the temperature change, and set it to isothermal. But the result is obviously wrong. The head is very high and the torque is wrong. The torque on the hub and rim is very large, accounting for about a quarter of the blade torque.The turbulence model is sst. Below is the cel expression for the water. LIBRARY: &replace MATERIAL: water com Material Description = Water (liquid) COM Material Group = Water Data,Constant Property Liquids Object Origin = User Option = Pure Substance Thermodynamic State = Liquid PROPERTIES: Option = General Material ABSORPTION COEFFICIENT: Absorption Coefficient = 1.0 [m^-1] Option = Value END DYNAMIC VISCOSITY: Dynamic Viscosity = 8.94E-4 [m^2 s^-1] *Density Option = Value END EQUATION OF STATE: Density = 997 [kg m^-3] + (Absolute Pressure-101325 [kg m^-1 s^-2])/(2.15e9 [m^2 s^-2]) Molar Mass = 18.02 [kg kmol^-1] Option = Value END REFERENCE STATE: Option = Automatic END REFRACTIVE INDEX: Option = Value Refractive Index = 1.0 [m m^-1] END SCATTERING COEFFICIENT: Option = Value Scattering Coefficient = 0.0 [m^-1] END SPECIFIC HEAT CAPACITY: Option = Value Specific Heat Capacity = 4181.7 [J kg^-1 K^-1] Specific Heat Type = Constant Pressure END TABLE GENERATION: Maximum Absolute Pressure = 1.0E6 [Pa] Minimum Absolute Pressure = 1000.0 [Pa] END THERMAL CONDUCTIVITY: Option = Value Thermal Conductivity = 0.6069 [W m^-1 K^-1] END THERMAL EXPANSIVITY: Option = Value Thermal Expansivity = 2.57E-04 [K^-1] END END END END Would you please let me know why this way of making the fluid slightly compressible causes serious problems? Many thanks in advance! |
|
May 2, 2024, 12:13 |
|
#2 |
Senior Member
Join Date: Jun 2009
Posts: 1,815
Rep Power: 32 |
Which equation of state is that one?
What boundary conditions are you using? Once it is not compressible, pressure boundary conditions level matters. That is not the case for incompressible fluid where the "delta" pressure is only thing that matters. List to check: 1 - Correct way to access pressure for material properties usage? 2 - Domain reference pressure? 3 - Since density is an expression, table generation settings? 4 - Boundary conditions levels with respect to the domain reference pressure
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum. |
|
May 2, 2024, 18:53 |
|
#3 |
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,728
Rep Power: 143 |
That is a bulk modulus EOS. It uses the bulk modulus of the material to slightly modify the density as a function of pressure. This is approach is typically used in things like water hammer.
Be aware that this is no longer an incompressible simulation. Obviously the density varies, so it is now compressible. This means that you get acoustic effects (pressure waves etc), and in water the speed of sound is around 1500m/s, so this frequently causes a severe restriction on the time step size. You usually need to use far finer time steps then incompressible simulations, and even finer than if you used an ideal gas model for air (the acoustic velocity of air is around 330m/s at atmospheric conditions). I would strongly recommend you to model this with a constant density fluid first, and get the simulation working accurately with constant density first. Then add the bulk modulus density function - you are probably going to have to make the time steps much finer, and possibly other convergence tricks will be required. But unless the basic simulation works and is accurate with an incompressible fluid you have no hope of getting it to work.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum. |
|
May 2, 2024, 21:53 |
|
#4 | |
New Member
Join Date: Jan 2022
Posts: 20
Rep Power: 4 |
Quote:
I am newer to the setting for the CFX software besides the basic setting. The boundary is shown below: Inlet: mass flow rate, outlet: static presure( 1atm) Domain reference pressure For TABLE GENERATION, only set the max/min pressure: Maximum Absolute Pressure = 7e+05 [Pa] Minimum Absolute Pressure = 4000 [Pa] From my limited experience, I thing static presure ought to 0 atm.Have a try. |
||
May 2, 2024, 22:00 |
|
#5 |
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,728
Rep Power: 143 |
As the EOS is linear table generation is normally OK, you just need to make sure you have enough range to cover the highest and lowest pressure you will ever encounter + a tolerance for numerical convergence.
What is the highest and lowest pressure you expect to see in this model? Is this a steady state or transient model? And as I said before - the most important thing is that this model runs OK and is accurate with a constant density material model before you apply the variable density model. Have you done this?
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum. |
|
May 2, 2024, 22:03 |
|
#6 | |
New Member
Join Date: Jan 2022
Posts: 20
Rep Power: 4 |
Quote:
The work set as constant density fluid is over, I wana discuss how the fluid slightly compressible will effect on internal flow field and pressure pulsation. Try finer time steps first. Thank you for your advice. |
||
May 2, 2024, 22:09 |
|
#7 |
New Member
Join Date: Jan 2022
Posts: 20
Rep Power: 4 |
It"s teady state.
The result set as constant density material model is ok. The max/min pressure is set as below and the pressure range is much wider than the real from the simulation of constant density. Maximum Absolute Pressure = 7e+05 [Pa] Minimum Absolute Pressure = 4000 [Pa] |
|
May 2, 2024, 22:43 |
|
#8 |
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,728
Rep Power: 143 |
On the constant density simulation, what are the maximum and minimum pressures the model predicts?
Please attach an output file from a variable density simulation.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum. |
|
Tags |
density correction |
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
[ICEM] ICEM Scripting Issues | tylerplowright | ANSYS Meshing & Geometry | 33 | September 27, 2021 16:35 |
Possible bug with stitchMesh and cyclics in OpenFoam | Jack001 | OpenFOAM Pre-Processing | 0 | May 21, 2016 08:00 |
correction of Grub after installing Windows XP and 8 | immortality | Lounge | 20 | January 5, 2014 17:41 |
[snappyHexMesh] determining displacement for added points | CFDnewbie147 | OpenFOAM Meshing & Mesh Conversion | 1 | October 22, 2013 09:53 |
Result is not correct | Li | FLUENT | 1 | December 30, 2000 00:21 |