CFD Online Discussion Forums

CFD Online Discussion Forums (
-   STAR-CCM+ (
-   -   Numerical Towing Tank Velocity Ramp (

lava12005 July 30, 2012 23:52

Numerical Towing Tank Velocity Ramp
Hi all,

I am simulating a towing tank and would like to do a simulation where the model start from rest (0m/s) to a test speed, say 1m/s.
I would like to know on how to ramp up the velocity in using the VOF model?

I tried to do a simple simulation where there is no model at all, and using the boundary condition as those specified in the DFBI Boat tutorial. Except that I change the Velocity Magnitude boundary condition using a field function of $Time

I am using dt of 0.01s, so after one time step, I expect the speed in the whole domain should be 0.01 m/s. But it is not and even after 100 iteration it is not converging to 0.01m/s

Does anyone can help me in this?

sanjay July 31, 2012 03:17

Try to run for more iterations, 100 is too less.
I had carried out similar towing tank experiments for flow visualization, but didn't try numerical simulation of it. I am looking forward do the same :)


lava12005 July 31, 2012 03:29

Hi Sanjay, that 100 iterations is still within the 1 time step. Isn't is considered to be excessive already for just 1 time step?

Does it has something to do with the boundary condition? Maybe the hydrostatic pressure outlet doesn't really allow this? Any suggestion?

Sideshore July 31, 2012 04:12

I've done this in the past.

I've specified a velocity ramp at inlet boundary. And you need to add momentum to the fluid in the domain while accelerating the fluid.

Good luck!

ryancoe July 31, 2012 09:27

Sideshore is correct. You need to prescribe a motion to your body (and the domain surrounding it) not the flow at the inlet. Your setup is more akin to water tunnel increasing speed, than a carriage doing so.

You should be able to use a field function to set the time varying velocity of the body.

lava12005 August 17, 2012 00:27

Hi all,

Yes, thanks to the suggestion I manage to ramp the velocity on the domain (just a water channel without any object) by using the User Defined Vertex, grid velocity method and using the user field function to setup the time varying motion.

Now If I want to have an object being ramp by the carriage (free to heave and trim) is this still possible?
Normally for fixed speed, I create an Overset mesh and prescribed a DFBI rotation and translation to it, but I don't know how to ramp the velocity in this region (since we have prescribed the motion as DFBI).

Henry Arrigo September 5, 2012 06:13

You can start with a velocity namely 0.1 m/s and run the case until it converges. then stop the simulation and change the velocity to namely 0.2 m/s and then run the case again. try to repeat these sequences until you reach the 1 m/s.
or if you have any idea about the needed power at 1 m/s you can use the thrust power instead of velocity.

lava12005 September 14, 2012 11:15

I finally able to do it via adding gravity in the flow direction (according to the ramping acc). Anyway just asking, if say we are using momentum source option (constant) to accelerate the fluid, but since there is 2 diff fluid here (air and water) doesn't it makes the air is accelerated more than the water?

Sideshore September 17, 2012 03:03

You have to make the force you apply dependent on the mass you want to accelerate.

I think in Star-ccm+ you define a volumetric momentum force. So the force applied to each cell does not automatically depend on the mass in the cell. You can use the volume fraction to calculate the mass in the cell.

All times are GMT -4. The time now is 23:49.