simpleFoam - pressure (coefficient) of head shape

GJM1991 · May 7, 2015, 04:38

Gents,

I am currently doing my thesis on cavitation modelling and with that reason I started using openFOAM.
The solvers I am using (cavitatingFoam and simpleFoam) are working just fine but the resulting pressure (and thus pressure coefficient) I am obtaining with simpleFoam are not even close to the values found in literature and by other CFD-papers.
What I am trying to do is study cavitation behaviour of a 'hemispherical head', this case has a lot of experimental data by Rouse & McNown (see attached picture of Cp-plots) and it indicates that the pressure coefficient should be around 1.00 on the nose and about -0.75 for the lowest pressure. This is also confirmed by a thesis written by R.W. Erney (see attached picture of pressure field around head shape) who also used simpleFoam to verify the single phase (without cavitation) pressure coefficient and finds high value for pressure: 37.11 and low value for pressure: -24.76. This comes close to the experimental pressure coefficient knowing that the free stream velocity is around 8.27 m/s.

In my simulation I have setup a case with boundary conditions identical to the case simulated by R.W. Erney. The simulation runs fine, converges to stable low residuals (1e-5 - 1e-6), the domain itself I sufficiently large to assume free stream values, but the pressure field is nowhere near the correct values (high: 38.95, low: -48.64). After that I did another run without a turbulence model, but the pressure field did not change significantly (high: 37.31, low: -51.47). There must be something small and simple I'm overlooking, but for now I am completely stumped...

I included some additional sketches of my problem and provided a link to the complete case in a rar-file and a link to the thesis by R.W. Erney. Could somebody please take the time to look at my case and tell what error(s) this novice has made? You would totally make my week!

THESIS BY R.W. ERNEY

OPENFOAM CASE FILE

taxalian · May 8, 2015, 16:37

Having a first look at your problem, even in the thesis by R.W. Erney, the pressure coefficient shown in Fig.5.17 is not really 1 at the nose of the body, both the turbulence model over-predicted the Cp. Secondly, looking at the Cp contour plot this is just a post-processing stuff, you can also adjust your contour levels accordingly as shown in thesis.

One more essential thing, it has been mentioned in the thesis work at Page 52, that the mesh has a yPlus value around 1. That is not the case in your mesh, see the yPlus output for your mesh below:

Patch 3 named cylinder y+ : min: 75.6029 max: 173.664 average: 104.528

this would also make a difference in your results.

My advice would be to perform a grid independent study for your case, that will help you in your thesis.

Anyway, i am having a look at your test case and let you know if i will be able to solve your issues.

GJM1991 · May 9, 2015, 09:19

Dear sir,

First of all, thank you very much for you time and effort, it is much appreciated!
Currently I am trying something in a different direction, the fact that the headshape is spherical got me thinking about the difference between the pressure distribution on a sphere and an (infinitely) long cylinder.
The mesh I have now is is not curved in the other plane, it is only a simple 2D-mesh. So now I am trying a small 3D-wedge to capture the curvature in the other direction.

If I find an answer I'll be sure to post it!

GJM1991 · May 11, 2015, 09:48

Quick update:

I have largely solved the problem by making it axi-symmetric instead of a 2d model. Basically I was looking a the pressure distribution of a cylinder, not at the pressure distribution of a sphere, which is curved in two planes. So by creating a wedge-shaped mesh instead of a flat (1 cell deep) mesh I solved my problem.

@taxalian

I would still be very appreciated if you can offer some advice on the meshing of the model to improve the quality of the turbulence modeling. Do keep in mind that I'm using wall-models so am I correct that the Yplus-value can be kept well above 1? I could be wrong, but isn't it true that most wall-models shouldn't be used below Yplus-value of 11? Because at that point you're basically trying to fully capture the turbulence in your mesh... right?

taxalian · May 12, 2015, 17:15

It's good to hear that you are progressing in the right direction. Related to the wall function, its ok that if you use higher values of y+ like 20, 30, 50 etc. If you want to resolve till the wall then you need to use low-Re turbulence model with appropriate scalable wall function on the expense of computational cost.

Anyway, i will let you know if i get some better results with two dimensional mesh.

May 7, 2015, 04:38	simpleFoam - pressure (coefficient) of head shape	#1
GJM1991 New Member Gert-Jan Meijn Join Date: Apr 2015 Posts: 8 Rep Power: 10	Gents, I am currently doing my thesis on cavitation modelling and with that reason I started using openFOAM. The solvers I am using (cavitatingFoam and simpleFoam) are working just fine but the resulting pressure (and thus pressure coefficient) I am obtaining with simpleFoam are not even close to the values found in literature and by other CFD-papers. What I am trying to do is study cavitation behaviour of a 'hemispherical head', this case has a lot of experimental data by Rouse & McNown (see attached picture of Cp-plots) and it indicates that the pressure coefficient should be around 1.00 on the nose and about -0.75 for the lowest pressure. This is also confirmed by a thesis written by R.W. Erney (see attached picture of pressure field around head shape) who also used simpleFoam to verify the single phase (without cavitation) pressure coefficient and finds high value for pressure: 37.11 and low value for pressure: -24.76. This comes close to the experimental pressure coefficient knowing that the free stream velocity is around 8.27 m/s. In my simulation I have setup a case with boundary conditions identical to the case simulated by R.W. Erney. The simulation runs fine, converges to stable low residuals (1e-5 - 1e-6), the domain itself I sufficiently large to assume free stream values, but the pressure field is nowhere near the correct values (high: 38.95, low: -48.64). After that I did another run without a turbulence model, but the pressure field did not change significantly (high: 37.31, low: -51.47). There must be something small and simple I'm overlooking, but for now I am completely stumped... I included some additional sketches of my problem and provided a link to the complete case in a rar-file and a link to the thesis by R.W. Erney. Could somebody please take the time to look at my case and tell what error(s) this novice has made? You would totally make my week! THESIS BY R.W. ERNEY OPENFOAM CASE FILE

May 8, 2015, 16:37		#2
taxalian Senior Member Join Date: Nov 2010 Posts: 139 Rep Power: 15	Having a first look at your problem, even in the thesis by R.W. Erney, the pressure coefficient shown in Fig.5.17 is not really 1 at the nose of the body, both the turbulence model over-predicted the Cp. Secondly, looking at the Cp contour plot this is just a post-processing stuff, you can also adjust your contour levels accordingly as shown in thesis. One more essential thing, it has been mentioned in the thesis work at Page 52, that the mesh has a yPlus value around 1. That is not the case in your mesh, see the yPlus output for your mesh below: Patch 3 named cylinder y+ : min: 75.6029 max: 173.664 average: 104.528 this would also make a difference in your results. My advice would be to perform a grid independent study for your case, that will help you in your thesis. Anyway, i am having a look at your test case and let you know if i will be able to solve your issues. Last edited by taxalian; May 12, 2015 at 17:16.

Thread Tools	Search this Thread
Show Printable Version Email this Page	Search this Thread: Advanced Search
Display Modes
Linear Mode Switch to Hybrid Mode Switch to Threaded Mode

Similar Threads
Thread	Thread Starter	Forum	Replies	Last Post
Simulation of a single bubble with a VOF-method	Suzzn	CFX	21	January 29, 2018 00:58
sonicFoam - pressure driven pipe: flow continuity violation and waveTransmissive BC	Endel	OpenFOAM Running, Solving & CFD	3	September 11, 2014 16:29
Contour of Pressure Coefficient and Velocity Vectors Colored by Pressure Coefficient	sonam	OpenFOAM	0	August 2, 2012 00:16
pressure ratio simpleFoam boundary case/0/p	Hasselhoff	OpenFOAM	2	June 29, 2009 18:43
Hydrostatic pressure in 2-phase flow modeling (long)	DS & HB	Main CFD Forum	0	January 8, 2000 15:00

May 9, 2015, 09:19		#3
GJM1991 New Member Gert-Jan Meijn Join Date: Apr 2015 Posts: 8 Rep Power: 10	Dear sir, First of all, thank you very much for you time and effort, it is much appreciated! Currently I am trying something in a different direction, the fact that the headshape is spherical got me thinking about the difference between the pressure distribution on a sphere and an (infinitely) long cylinder. The mesh I have now is is not curved in the other plane, it is only a simple 2D-mesh. So now I am trying a small 3D-wedge to capture the curvature in the other direction. If I find an answer I'll be sure to post it!

May 11, 2015, 09:48		#4
GJM1991 New Member Gert-Jan Meijn Join Date: Apr 2015 Posts: 8 Rep Power: 10	Quick update: I have largely solved the problem by making it axi-symmetric instead of a 2d model. Basically I was looking a the pressure distribution of a cylinder, not at the pressure distribution of a sphere, which is curved in two planes. So by creating a wedge-shaped mesh instead of a flat (1 cell deep) mesh I solved my problem. @taxalian I would still be very appreciated if you can offer some advice on the meshing of the model to improve the quality of the turbulence modeling. Do keep in mind that I'm using wall-models so am I correct that the Yplus-value can be kept well above 1? I could be wrong, but isn't it true that most wall-models shouldn't be used below Yplus-value of 11? Because at that point you're basically trying to fully capture the turbulence in your mesh... right?

May 12, 2015, 17:15		#5
taxalian Senior Member Join Date: Nov 2010 Posts: 139 Rep Power: 15	It's good to hear that you are progressing in the right direction. Related to the wall function, its ok that if you use higher values of y+ like 20, 30, 50 etc. If you want to resolve till the wall then you need to use low-Re turbulence model with appropriate scalable wall function on the expense of computational cost. Anyway, i will let you know if i get some better results with two dimensional mesh.