[ghost82]

Originally Posted by darkluix88

This one probably is the better solution, applying the force to the centroid of the mass of fluid in tank.
Can you help me to create a simple UDF with the DEFINE_SOURCE macro?
For example, I want to use a simple sinusoidal velocity to the fluid: v=-omega*A*sin(omega*t + phase)
Because I'm a newbie and I don't understand some commands as C_R(c,t) or C_U(c,t), or the "con" variable.

You will not apply a force to the centroid of the mass: you define the source (which is in this case expressed in N/m3) in one or more zones and every cell in that zone(s) is subjected to that source.
So first thing is to calculate the function source you want to apply inside the tank, something like source=f(time, other variables you want to include), expressed in N/m3.
Then, I suggest to read the fluent udf manual and look at examples.
Macros such as C_R(c,t) and C_U(c,t) are described in the udf user manual.

[darkluix88]

Thanks for the help and I'm sorry for the too many questions that I ask you
Ok, I'm reading the manual and approaching to create the source file udf but I'm probably getting wrong...actually my code is this one for example:

#include "udf.h"
#define w 1
#define a 0.1
#define ph 0

DEFINE_SOURCE(xmom_src,c,t,dS,eqn)
{
real source;
real time=RP_Get_Real("flow-time");

if (time < 5)
{
source = -w*a*sin((w*time) + ph);
dS[eqn] = -w*w*a*cos((w*time) + ph);
}
else
source = 0;

return source;
}

I've set as constants the initial phase (0), omega (1) and amplitude (0.1) and the time step size as 5 seconds.
Which corrections have I to add for my purpose?

[ghost82]

The "source" in your udf must have unit N/m3 (force/volume): did you check it?
dS[eqn] is derivative of "source" in respect to the dependent variable of the transport equation (v(x)): did you check it?
Even if time >5 you have to assign dS[eqn].

What do you mean by "initial phase"?

[darkluix88]

How can I convert a sinusoidal velocity to N/m3? The only parameters known are these ones: amplitude, phase and pulsation (or frequency, is the same).
The initial phase is the delay/advance ("ritardo/anticipo") regarding the start position of the sine curve.

[ghost82]

Answers to your questions are partially in the post I reported.

More into details N/m3 is a force in respect to a volume and it's expressed in SI units as (kg*m/s2)*(1/m3).
This is the same as multiply acceleration (m/s2) by density (kg/m3).
If you have the velocity you can calculate the function for acceleration: accelaration is the variation of the velocity in respect to time, in other words simply d(velocity)/d(time).
Then calculate dS as I wrote.

So what you have to do is to define two udf: one for x momentum source, with acceleration function that multiply density (C_R(c,t));
one for y momentum source, with gravity force that multiply density.

Otherwise, only one udf for x momentum source, but enbable in fluent gui gravity in (-)y direction.

[darkluix88]

Okok, now I've understood how to approach the problem better!
So, at first I've to convert the physical quantity that I want to apply in momentum as N/m3, next I define the variable "source" as the quantity previously calculated, and at last "dS[eqn]" represent the derivative of the "source" respect to the velocity...is it right?
I've modified the udf code as this one:

#include "udf.h"
#define w 1
#define a 0.1
#define ph 0

DEFINE_SOURCE(xmom_src,c,t,dS,eqn)
{
real source;
real time=RP_Get_Real("flow-time");

if (time < 5)
{
source = (-w*w*a*cos((w*time) + ph))*C_R(c,t);
dS[eqn] = w*cot((w*time) + ph)*C_R(c,t);
}
else
source = dS[eqn] = 0.;

return source;
}

Are there errors in the formulas?
The input quantity is the same sinusoidal velocity: v(t)=-w*a*sin((w*t)+ph)...thanks for the help

[ghost82]

Equation for x momentum source seems correct to me.
dS[eqn] is dS/d(vx) so in my opinion it should be 0.

source = dS[eqn] = 0.;

Not sure you can do it in C; if not, write 2 lines instead of one.

[darkluix88]

Ah okok, I thought that dS[eqn] was different to 0 because, being the source (acceleration)*(density) and acceleration = (velocity/time), it contains the velocity expression inside of it...essentially I have multiplied and divided the source expression for " sin((w*time) + ph) " to point out the velocity expression.

[ghost82]

Maybe you are right, but I'm not 100% sure. Maybe someone else knows.
If it is right, use 1/tan instead of cot.

[darkluix88]

I've tried this type of udf and it works! Only I've explouted the cotangent expression because in udf cotangent command isn't detectedby fluent. Thanks for your help
Now I wanna use for example angular velocity, but I think that this approach "cell to cell" isn't optimal in this case, because effects as centrifugal and coriolis forces are neglected...

So how can I resolve this problem?

If I would use newly the Dynamic mesh, is it possible applicate the force/movement (translational or angular) to the tank, and so to the water, without deforming the cells?
Essentially: the water inside the tank moves, but the initial quad-cells of the tank don't deform. It would be a more precise model

[ghost82]

Yes, I just commented the above post for cot

Why are you saying centrfugal and coriolis forces are neglected?
As far as I know these forces are automatically calculated: you have to define the center and the axis of rotation in the fluid zones.

[darkluix88]

Exactly, I didn't notice it!

So are considered all the forces related to the movement imposed? I thought that the effect of coriolis (as centrifugal/centripetal effects) should be an effect regarding the entire structure, not the single cells...but I'm not sure of this.
So applying this method to rotational method is reliable? For the udf setting, I can use the same structure of previous code changing constants, source and dS[eqn] terms, right?

To have a complete control of the problem, is it possible to apply the dynamic mesh to move the tank without deforming the cell's geometry?

[ghost82]

So are considered all the forces related to the movement imposed?

Yes, I think so..

So applying this method to rotational method is reliable?

Try it

For the udf setting, I can use the same structure of previous code changing constants, source and dS[eqn] terms, right?

Yes

To have a complete control of the problem, is it possible to apply the dynamic mesh to move the tank without deforming the cell's geometry?

If you look at the sketch I posted some posts above the cells of the tank will not be deformed; new/old layers of cells will be added/removed outside of the tank, but you are not interested in the outer domain, so you can fill the outer domain with air and assign a P inlet/P outlet condition.

However I think the best solution is to apply sources to momentum equation.

[darkluix88]

Okok, I will try this approach to various cases and I'll let you know

Now I've understood, but I've to set a particular condition to avoid the cell's deformation with this scheme or it's automatic after created the outer domain?
Are static also the upper and bottom walls of the outer domain, or only its left and right walls as in the sketch?
Another idea: is it possible to extend the outer domain also up and down respect to the tank? So simultaneously I could apply more velocity vectors (for example) in different directions without the problem of cell's deformation.

[ghost82]

Originally Posted by darkluix88

Okok, I will try this approach to various cases and I'll let you know

Now I've understood, but I've to set a particular condition to avoid the cell's deformation with this scheme or it's automatic after created the outer domain?
Are static also the upper and bottom walls of the outer domain, or only its left and right walls as in the sketch?
Another idea: is it possible to extend the outer domain also up and down respect to the tank? So simultaneously I could apply more velocity vectors (for example) in different directions without the problem of cell's deformation.

To avoid deformation you have to set rigid body motion to the interior of the tank also (not only the walls), so you will apply motion to walls and to interior of the tank.
You can extend outer domain the way you want.

[darkluix88]

Hi ghost82, I ve tried these days applying dynamic mesh with walls as rigid body and also the default_interior as rigid body, but it doesn't run.
In fact the tank moves but the fluid inside remain at the initial relax position with no sloshing...how can I resolve the problem? Thanks for the help

[ghost82]

I have to try, not soon, but I'll let you know.
You can try to set as rigid body not the default interior but the fluid zone name.

[darkluix88]

I obtain the same result....ok thanks, for now I post newly the question because I have to go on with my thesis

[darkluix88]

Hi ghost82, returning to the momentum source method to simulate sloshing, how can I write the udf for the rotation source, defining the centre of rotation and the axis? For example, if I want apply the rotation to the centroid of the tank, which commands I've to use?

[ghost82]

Hi!
I think that if you want to simulate rotation around a central axis of a 2d rectangle you are assuming a cilindrical tank.
If this is not your case I think you have to simulate a 3d geometry.
I think there's no need to write udf if your tank rotates at a constant angular velocity (here you simulate steady state solution): assuming your rectangle is centered in xy plane, set up your case with gravity in -y direction and you're ready to go.
If you want to do a transient simulation then angular velocity starts from 0 rad/s and reach xx rad/s, so you have equation for angular velocity in respect to time; so, follow what you have done for translational motions.

This is for axisymmetric:
http://aerojet.engr.ucdavis.edu/flue...ug/node399.htm