General momentum source
 

hi everyone
I am trying to simulate propeller behind the hull as a actuator disk. From literature and posts from this forum i came to know that this can be achieved using an actuator disk without simulating the actual propeller.
my purpose is to find the wake in front of the disk. For that i created a subdomain which is assigned as a 3D momentum source. I followed the tutorials for this.
now i want to assign the axial and radial accleration to the disk. does anybody knows how do i do this?
i tried using zero values for momentum source the flow pattern was good. when i use some constant value for momentum source, the flow pattern is not as expected.
Does any body know how to write CEL for velocity which is varying with radius from disc center to tip?
i was trying writing but always getting syntax error.
please help me. i m in need.
thanks in advance

"Wake in front of the disk".... I don't get that. How can a propeller which generates thrust have a wake in front of the prop? Isn't the water just sucked into the prop disk?

CEL (assuming the prop rotates along the x axis):
radius = sqrt ( y*y + z*z)
Flow = radius * 10 [apprpriate units for your source term]

The the variable Flow will be 10*the radius. So you can set it to any function of radius you like from there.

General momentum source
 

Thanks Ghorrocks for your quick and kind reply.
"wake in front of the propeller" here indicates the the flow from ship hull bottom sucked into the propeller. i have attached the a picture of the expressions used for momentum source. i have imported radial variation of axial and rotational velocity as functions and then defined a additional variable called"StepRotor". Now when i want to use that variable in the expressions along with the function; the CFX is showing error as "unrecognised names" or the name is already used. i wanted to know how to use function and variable while writing expression for general momentum source. Can u suggests me something?
waiting for your reply.
thanks in advance

The unrecognised names error simply means you need to be referencing the correct objects. If you cannot fix this error then post the output and we can give it a go for you.

general momentum source
 

@ghorrocks
i am not getting what do you mean by correct objects. Without fixing this error i can't able to run the program.

It would probably be best if you posted the output file which shows the error message, and includes your CCL.

i am not getting error in output but in CFX Pre itself. while writing the expression for Fn(refer to earlier post) i am getting an error as
"Bad expression value 'Fn volume' detected in parameter 'Momentum Source X Component' in object '/FLOW:Flow Analysis 1/DOMAIN:Domain 1/SUBDOMAIN:Subdomain 1/BULK SOURCES/MOMENTUM SOURCE/GENERAL MOMENTUM SOURCE'.
CEL error:
The following unrecognised names were referenced: axial vel, subdomain 1."

i have attached the output file.

The name "StepRotor" is used for a CEL expression and your AV name. This is a really bad idea - parsers get very confused with this. There may be others, I did not check in detail. Make sure all expressions and defined names are unique.

general momentum source
 

Dear Ghorrocks thank you for your suggestions. I corrected the errorrs. That is due to same nomenclature used in AV and expressions.

now i can give the momentum source for subdomain. for acuator disk i have imported axial and rotational velocities as functions. they vary with the radial location of the disk from the center of the disk. i want to include the rotation effect of the disk to the momentum source. i tried including but not getting the helical pattern of the flow downstream of the disk as it should be. i am using cartesian coordinate system. i used following expressions:
CEL:
EXPRESSIONS:
Fn volume = StepRotor*((den*Volume force domain*((va)/tstep))/Volume \
force domain)
Fy = StepRotor*((den*Volume force domain*((omega*r)/tstep))/Volume \
force domain)
Fz = StepRotor*((den*Volume force domain*((vr*omega*r)/tstep))/Volume \
force domain)
Rrotor = 1000[m]
StepRotor = StepRotorRad*StepRotorX
StepRotorRad = step((Rrotor-sqrt(r^2))/1[m])
StepRotorX = step(x/1[m])*step((Xdisc-x)/1[m])
StepRotorY = step(y/1[m])*step((Ydisc-y)/1[m])
StepRotorZ = step(z/1[m])*step((Zdisc-z)/1[m])
Volume force domain = 2*pi*sqrt((y+7315[m])^2+(z-1300[m])^2)*dr*Xdisc
Xdisc = 500[m]
Ydisc = 1000[m]
Zdisc = 1000[m]
den = 1025[kg m^-3]
dr = 0.1[m]
hw = 4853[m]
omega = 100 [rad s^-1]
rrotor = 0[m]
tstep = 1[s]
va = axial vel(r)*StepRotor
vfair = 1-vfwater
vfwater = step((hw-z)/1[m])
vr = rotational vel(r)*StepRotor


can anybody tell me where i went wrong?

Can you show an image of what you are getting?

i attached the streamline pattern image. the streamlines are straight before and after the disc.
please help

I do not have time to debug your equations - but I can see your "Fn volume" equations are wrong - the Volume force domain just cancels out as they are currently written.

@ Ghorrocks
thanks for your reply.
i used F=density*volume of the disc*velocity/time step
for that i calculated volume of the disc at each radial location and as cfx wants force per unit volume, i divided that force with volume of the disc.

If you are looking for a spiral flow then I would expect to see something like:
Fy = a * z
Fz = -a * y

I do not see Fy has any z term in your equation, nor has Fz has any y term. So you are missing these terms.

general momentum source
 

Dear Ghorrocks
i tried what u suggested. it was helpfull for me. i used following expressions
Faxial = -den*axial vel /tstep
Ftangential = -den*tangential vel*100[rad s^-1]

for a disk in single phase simulation i was getting very nice and anticipated flow through the disk but when i use same expressions for the disk behind the hull case i m ending with some nonsense flow pattern as i posted earlier.

i am confused why these expressions works in single phase of actuator disk simulation and fails in actuator disk behind the ship hull case.
could you please suggest me how i can improve the modelling?
waiting for reply
:)

hi everyone
referencing to my previous post i am trying to simulate propeller behind the ship hull using actuator disc concept. It is a multiphase flow problem.
i was able to simulate the disc in single phase domain but unable to simulate in multiphase doamin.

Can anybody would like to explain me why this is happening with me. I am in need. please help

Can you show what you are getting in the single phase and multiphase simualtion results? Some images would help. Also are you using homogenous or inhomogenous multiphase models?

general momentum source
 

hi
i attached the snap shots for single and multiphase streamlines. You can see in single phase the streamline rotates downstream of the disc as expected but in multiphase they do not.
i am using homogeneous multiphase(standard) model. If in case i has to use inhomogeneous model then please suggest how to do it.
the equations from the previous post were used in both cases.

If this is a free surface model with a coherent free surface then use the homogenous model.

You will need to do some basic fault finding - Is the disk above or below the water line? Is your free surface being resolved tightly? Is the velocity for both phases showing this trend?