CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   OpenFOAM Running, Solving & CFD (http://www.cfd-online.com/Forums/openfoam-solving/)
-   -   ComputeTorqueMRF probel (http://www.cfd-online.com/Forums/openfoam-solving/58480-computetorquemrf-probel.html)

 waynezw0618 October 3, 2008 11:31

Hi everyone i am use the sa

Hi everyone

i am use the same mesh to do the calculation of a pump impeller in CFX and OF1.4.1.But i got quiet different result of torque.

X CFX-SST OF-SST

torqueZ@shroud -0.0161 -0.16478

would any one could tell what is wrong with my reuslt? for at blade.one is negative and one is positive?and for at shroud the OF value is too large which will cause the shaftpower to zero to sum from all rotation part.

any way the basic result was quiet simimlar as shown in p for both
CFX result
http://www.cfd-online.com/OpenFOAM_D...ges/1/9427.png

 waynezw0618 October 3, 2008 11:33

OF result http://www.cfd-onli

 hani October 3, 2008 16:15

Hi Wayne, How do you comput

Hi Wayne,

How do you compute the torque? If your pressure fields are this similar you should get quite similar torques as well. I'd say that there is a problem with your torque calculation.

Håkan.

 waynezw0618 October 4, 2008 01:08

Hi Hakan I compute the torq

Hi Hakan

I compute the torque by using the application of computeToqueMRF from openfoamwiki.

 hani October 4, 2008 04:00

Hi Wayne, I have never used

Hi Wayne,

I have never used that application myself. I would recommend that you check that r0 is evaluated correctly, and that all the required patches are used. Then you should not use this code in parallel, since the sum function only works in serial. Use the gSum function in parallel.

Håkan

 waynezw0618 October 4, 2008 08:41

Hi Hakan i calculated the tor

Hi Hakan
i calculated the torque in the serial way.and i will see the code. i have two question.

1) what is r0?how to evaluate the r0?

2) would you mind to give me some idea to calculate the torque of pump impeller.i find the model error is too large for log-law wall function especially in the off-design condition.i think that because of the log-law is not of the physical in the rotation frame. which turbulence model or wall function is suitable to precisely calculate the torque of impeller ?

thanks

yours wayne

 hani October 4, 2008 15:10

Hi Wayne, Just by looking a

Hi Wayne,

Just by looking at the code it looks like r0 is a reference point that should be located at the axis of rotation. It is used to calculate the distance from the axis of rotation to each face that contributes to the torque. In computeTorqueMRF it looks like it is calculated automatically, but since you experience some problem, you should check that it is done correctly, and that you have your case set up correctly.

For the torque you have two contributions, from the static pressure and from the viscous forces. The static pressure forces are the dominant. You should not bother about turbulence models or wall functions at the moment. You should focus on verifying the postprocessing. Your static pressure field looks fine, so your torque should be fine as well. The torque is given by the sum over all faces, of the static pressure times the face area times the radius of the center of each face.

Håkan.

 waynezw0618 October 6, 2008 05:27

Hi Hakan thanks a lot! i

Hi Hakan

thanks a lot!

i think there may be a bug in the computeTorqueMRF as:

torque = sum((cPatch.Cf()-r0)^((p.boundaryField()[patchID]*1000+pref)*cPatch.Sf()))

where scalar pref = 101325.0;

and the red part is which i think should be added on for the dimension of p in MRFSimpleFoam is without density of fluid.here i use 1000 for density of water.is that right?

but the result is quiet different from CFX:

X OpenFOAM-1.4.1-SST CFX-standard k-e CFX-SST CFX-LES

torqueZ@shroud -0.144787 -0.01041 -0.01161 -0.0317

1)the torque at shroud is too large.as you mentioned the torque have two contributions, from the static pressure and from the viscous forces.and the computeTorqueMRF do not calculate the contribution of viscous.so the pressue at shroud should not contribute to the torque,for the p is normal to the shroud and the component is either normal or parallel to the normal to the axial.so the torque contributed by pressure at shroud be zero by using computeTorqueMRF. and the visous`s contribution is very small.and it is clearly in all CFX result,for i guess this value is just contributed from viscous.

2) the torque at blade is too small.i guess that is because of the contribution of viscous at blade was not calculated.for the resistance should be very large at the off-design condition.

is that right?

by the way,of question last time.i mean the viscous`s contribution to the torque maybe quite small in pump`s design condition,but it will be greater in the off-design condition for two way.one is that,at off-design condition there will be flow separation,and the vortex resistance is larger than at the design condition(which will almost zero),so the direct contribution of viscous will increase. the other is that with the vortex in the impeller passage the follow pattern is complex than at the design condition so the torque contributed by the pressure is not change linear with Head of pump,so the efficiency will decrease.any way both two was affect torque calculation by vortex which is related to the viscous.and i have done some validation and verification study of pump impeller calculation in ANSYS CFX with standard k-e model and Menter`s SST model.and i find that, quite different from the design condition,although the flow pattern should be calculated very close to the PIV meassurement, the velocity profile can`t predict well.and i will post that later on.and it is like the calculation of airfoil,the flow separation(especially the separation point) is not well calculated.so i think the viscous effect to the torque is important. i dont know if it is right. would you mind to give me some advices.

thanks

yours wayne

 waynezw0618 October 6, 2008 05:34

follow pattern of ANSYS-CFX with standard k-e

http://www.cfd-online.com/OpenFOAM_D...ges/1/9446.gif

 waynezw0618 October 6, 2008 05:42

follow pattern of ANSYS-CFX with standard k-e with finer mesh

http://www.cfd-online.com/OpenFOAM_D...ges/1/9449.gif

 waynezw0618 October 6, 2008 05:49

follow pattern of ANSYS-CFX with Mentors`SST with finer mesh

http://www.cfd-online.com/OpenFOAM_D...ges/1/9451.gif

 waynezw0618 October 6, 2008 06:08

Velocity profile calculation o

Velocity profile calculation of standard k-e at r/R0=0.5 of 4 different grid(constant mesh refinement ratio r=1.2 )

up is Wt(tangential velocity) down is Wr(axial velocity),left is design condition,right is off-design conditon

http://www.cfd-online.com/OpenFOAM_D...ges/1/9453.gif

the pump geometry and PIV result is info to reference [1]

mesh refine is info to reference [2]

reference
[1]Nicolas Perdeson,etc.Flow in a Centrifugal pump impeller at design and off design condition-Part I:Particle Image Velocity(PIV) and Laser Dopper Velocimetry(LDV)meassurement,[J]J.fluid.Eng. 2003,Vol125,p61-72.

[2]Fred Stern,Rober V. Wilson,etc.Comprehensive Approach to Verification and Validation of CFD simulation-Part 1: Methodology andProcedures[J]J.fluid.Eng. 2001,Vol123,p793-803

 waynezw0618 October 7, 2008 02:56

Hi Hakan would you mind gi

Hi Hakan

would you mind give me some adviseï¼Ÿ

I have convert the OF result to fluent data,and calculate the torque in fluent.and also no viscous forces.the value is:

torqueZ@shroud 0.0200

thanks

yours wayne

 waynezw0618 October 7, 2008 03:37

torqueZ@shroud 0.0200

this value by postprocessing the OF result in Fluent

regard

wayne

 waynezw0618 October 8, 2008 10:29

Hi Hakan i have studied the

Hi Hakan

i have studied the code of computerTorqueMRF for two days.but i still cannot find the problem,would you mind help me ?

thanks!!

wayne

 dmoroian October 9, 2008 01:55

i think there may be a bug in

Quote:
 i think there may be a bug in the computeTorqueMRF as: torque = sum((cPatch.Cf()-r0)^((p.boundaryField()[patchID]*1000+pref)*cPatch.Sf())) where scalar pref = 101325.0; and the red part is which i think should be added on for the dimension of p in MRFSimpleFoam is without density of fluid.here i use 1000 for density of water.is that right?
Hello Wayne,
Indeed, I did not take into account different densities, and I tested the utility only on air!!!
As you probably know, when you use an incompressible solver, the pressure is not actually the pressure but is the ratio between pressure and density. However, when using air, the OpenFOAM tutorials consider density 1 kg/m3, hence the absolute value of the ratio will be the same with the static pressure (but different units).
So, to be correct, in your case, you should multiply the pref with 1000:
torque = sum((cPatch.Cf()-r0)^((p.boundaryField()[patchID]+pref)*1000.0*cPatch.Sf()))
I have a newer version of the utility (including gSum as Hakan suggested), which I will modify to account for different densities of the fluid.

Dragos

 waynezw0618 October 9, 2008 13:13

Hi Dragos thanks to your re

Hi Dragos

i am sorry for i still can not understand why you mulityply pref with 1000 because i guess as you define the pref equal to the 101325,you assume the dimension of pre is pa,and pre is enviromental pressure.an 1000 is refer to the density of water- 1000kg/m^3.and as a result, each value in the first table of this topic will multiply with 1000(i have tried).that was too large,and it is larger and larger than the result of CFX and experiment.

and would you mind to tell me how to add the viscous effect to the torque. because as my result with CFX (both ke,SST,LES), the viscous effect to the torque at the shroud is very large,and it is about 0.02-0.07 of pressure effect at blade.so i do`t think it could be ignored.considering the comparing error between CFD and experiment result is about such level.

thanks

 dmoroian October 10, 2008 02:47

Well, I think this is a matter

Well, I think this is a matter of ... taste, but definitely if you consider pref [Pa], then there is no reason for it to be multiplied by density, so your formula is correct.
I'll have to think about the wall shear stress implementation in the torque computation.
In the mean time can you tell me what kind of boundary conditions do you have? I'm asking because I'm trying to compute a 2 stage axial compressor, and I cannot make the flow to go the right direction, it always goes backwards.

Dragos

 waynezw0618 October 10, 2008 10:49

Hi Dragos i am using the ve

Hi Dragos

i am using the velocity inlet before. but there is something wrong with result my velocity profile is no axial symmtry but it can`t see clearly in floor 2 of this topic.you can`t see from this picture.it will clearly with velocity profile ploting. i will show you later for i am away from office.

thanks

yours wayne

 All times are GMT -4. The time now is 08:24.