
[Sponsors] 
Pressure drop consistently lower than measured with SimpleFoam 

LinkBack  Thread Tools  Search this Thread  Display Modes 
March 2, 2021, 15:38 
Pressure drop consistently lower than measured with SimpleFoam

#1 
New Member
Join Date: Feb 2020
Posts: 6
Rep Power: 5 
I'm trying to simulate the pressure drop through a small rectangular duct with a 90 degree bend. I've measured the pressure drop at 70m^3/h to be around 165Pa but my simulations are always 5060Pa lower than that. Hopefully someone can see what I'm doing wrong. Am I defining a boundary condition incorrectly?
Control Dict Code:
application simpleFoam; startFrom startTime; startTime 0; stopAt endTime; endTime 2000; deltaT 1; writeControl timeStep; writeInterval 100; purgeWrite 0; writeFormat ascii; writePrecision 6; writeCompression off; timeFormat general; timePrecision 6; runTimeModifiable true; functions { #includeFunc streamlines } Code:
ddtSchemes { default steadyState; } gradSchemes { default Gauss linear; } divSchemes { default none; div(phi,U) bounded Gauss linearUpwind grad(U); div(phi,k) bounded Gauss limitedLinear 1; div(phi,epsilon) bounded Gauss limitedLinear 1; div(phi,omega) bounded Gauss limitedLinear 1; div(phi,v2) bounded Gauss limitedLinear 1; div((nuEff*dev2(T(grad(U))))) Gauss linear; div(nonlinearStress) Gauss linear; } laplacianSchemes { default Gauss linear corrected; } interpolationSchemes { default linear; } snGradSchemes { default corrected; } wallDist { method meshWave; } Code:
solvers { p { solver GAMG; tolerance 1e06; relTol 0.1; smoother GaussSeidel; } "(Ukepsilonomegafv2)" { solver smoothSolver; smoother symGaussSeidel; tolerance 1e05; relTol 0.1; } } SIMPLE { nNonOrthogonalCorrectors 2; consistent yes; residualControl { p 1e2; U 1e3; "(kepsilonomegafv2)" 1e3; } } relaxationFactors { equations { U 0.9; // 0.9 is more stable but 0.95 more convergent ".*" 0.9; // 0.9 is more stable but 0.95 more convergent } } Code:
transportModel Newtonian; nu [0 2 1 0 0 0 0] 1.516e05; Code:
simulationType RAS; RAS { // Tested with kEpsilon, realizableKE, kOmega, kOmegaSST, v2f, // ShihQuadraticKE, LienCubicKE. RASModel kOmegaSST; turbulence on; printCoeffs on; } Code:
dimensions [0 1 1 0 0 0 0]; internalField uniform (0.0 0.0 0.0); boundaryField { inlet { type flowRateInletVelocity; volumetricFlowRate 0.0194; value $internalField; } outlet { type zeroGradient; } wall { type noSlip; } } Code:
dimensions [0 2 2 0 0 0 0]; internalField uniform 0; boundaryField { inlet { type zeroGradient; } outlet { type fixedValue; value uniform 0; } wall { type zeroGradient; } } Code:
dimensions [0 2 2 0 0 0 0]; internalField uniform 0.3723; boundaryField { inlet { type fixedValue; value $internalField; } outlet { type inletOutlet; value $internalField; inletValue $internalField; } wall { type kqRWallFunction; value $internalField; } } Code:
dimensions [0 0 1 0 0 0 0]; internalField uniform 182.6; boundaryField { inlet { type fixedValue; value $internalField; } outlet { type inletOutlet; value $internalField; inletValue $internalField; } wall { type omegaWallFunction; value $internalField; } } Code:
dimensions [0 2 1 0 0 0 0]; internalField uniform 0; boundaryField { inlet { type calculated; value uniform 0; } outlet { type calculated; value uniform 0; } wall { type nutUSpaldingWallFunction; value 1e4; } } 

March 3, 2021, 05:02 

#2 
Senior Member
anonymous
Join Date: Jan 2016
Posts: 416
Rep Power: 13 
Hi!
What is your fluid? In simpleFoam p is a kinematic pressure (pressure/rho) so you will have to multiply the pressure drop with the fluid density to get the pressure in Pa. If you already did that, just ignore this reply. 

March 3, 2021, 08:21 

#3 
New Member
Join Date: Feb 2020
Posts: 6
Rep Power: 5 
Thanks I did make that mistake but I'm still out by a quite a bit after taking it into account. I ran the simulation again with the relaxationFactors brought down to 0.15 and the endTime extended to 10000. The pressure difference (attached) averages around 99. The fluid is air and the conditions during the measurement were Lab air Temp 19.2°C and Atmospheric Pressure 29.3 inHg so the density is around 1.18kg/m^3 I think. That means simpleFoam predicts the pressure drop as 99*1.18=116.82Pa at 70m^3/h while the measurement is 162m^3/h.
I'm running it again currently with a finer mesh to try rule that out as the problem. 

March 3, 2021, 08:26 

#4 
Senior Member
anonymous
Join Date: Jan 2016
Posts: 416
Rep Power: 13 
These residuals are quiet high and based on your attached file I would say that this simulation is not converged...


March 3, 2021, 08:43 

#5 
New Member
Join Date: Feb 2020
Posts: 6
Rep Power: 5 
Okay from reading other posts I had taught that it was because of the turbulence and once the residuals had leveled off it was as close as I'd get to converged. The finer mesh has just converged with a pressure difference of 93 (110Pa) at the last time step. I'll try lowering the residual controls to:
Code:
p 1e3; U 1e4; "(kepsilonomegafv2)" 1e4; 

March 3, 2021, 09:02 

#6 
Senior Member
anonymous
Join Date: Jan 2016
Posts: 416
Rep Power: 13 
It did not converged either.
Check your pressure. It is still increasing. For convergence you should check some physical values if they are not changing anymore, not the residuals. In your case you should run as long as your pressure drop is not changing anymore. 

March 3, 2021, 10:00 

#7 
New Member
Join Date: Feb 2020
Posts: 6
Rep Power: 5 
Thanks for the feedback, I've been focusing too much on the residuals. I'll work on getting results with a stable pressure result.


March 3, 2021, 12:37 

#8 
Senior Member
Join Date: Apr 2020
Location: UK
Posts: 570
Rep Power: 12 
The other thing to keep in mind is that you are being quite ambitious in trying to use CFD for this ... bear in mind that the pressure loss is all down to flow turbulence, and that the reason why the 90deg bend generates a larger pressure drop than a straight duct is because of flow separation and enhanced turbulence generation (which sucks energy out of the mean flow, ie the pressure field).
So, to get the correct pressure drop, you need to be able to model the smooth body separation and secondary flow patterns in the duct to high accuracy. This is not trivial! You will need a good mesh and a good turbulence model to get the answer spot on ... I don't want to dissuade you from trying, but do realise that this is not a trivial problem. Lastly  if you want to be ultra accurate  remember also that for simplicity, RANS solvers often combine the following two terms terms, into a single pressure gradient term, (the turbulence term is the contribution from the normal Reynolds stresses). The solver then solves for rather than for the static pressure , so for a true comparison you also ned to subtract off the turbulence energy part ... this is typically negligible though, which is why the approximation is made! Good luck. 

Tags 
duct, pressure drop, simplefoam 
Thread Tools  Search this Thread 
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
Pressure drop in pipe flow with Large Eddy Simulation  xerox  FLUENT  1  October 16, 2019 09:55 
OpenFOAM  cyclicAMI Pressure drop result variation  Vishsel  OpenFOAM  0  May 31, 2019 03:47 
total pressure and pressure drop  omaralyahia  CFX  5  July 14, 2015 09:13 
simpleFoam  pressure (coefficient) of head shape  GJM1991  OpenFOAM Running, Solving & CFD  4  May 12, 2015 18:15 
Hydrostatic pressure in 2phase flow modeling (long)  DS & HB  Main CFD Forum  0  January 8, 2000 16:00 