|
[Sponsors] |
July 30, 2012, 23:52 |
Numerical Towing Tank Velocity Ramp
|
#1 |
Senior Member
KHB
Join Date: Aug 2010
Location: Singapore
Posts: 118
Rep Power: 15 |
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? |
|
July 31, 2012, 03:17 |
|
#2 |
Member
aerosapien
Join Date: Sep 2010
Posts: 59
Rep Power: 15 |
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 regards www.aerosapien.blogspot.com |
|
July 31, 2012, 03:29 |
|
#3 |
Senior Member
KHB
Join Date: Aug 2010
Location: Singapore
Posts: 118
Rep Power: 15 |
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? |
|
July 31, 2012, 04:12 |
|
#4 |
New Member
Jan Willem Krijger
Join Date: May 2010
Posts: 8
Rep Power: 15 |
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! |
|
July 31, 2012, 09:27 |
|
#5 |
Member
Ryan Coe
Join Date: Jun 2010
Location: Albuquerque, NM
Posts: 98
Rep Power: 15 |
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.
__________________
Ryan |
|
August 17, 2012, 00:27 |
|
#6 |
Senior Member
KHB
Join Date: Aug 2010
Location: Singapore
Posts: 118
Rep Power: 15 |
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). |
|
September 5, 2012, 06:13 |
|
#7 |
Senior Member
Henry Arrigo
Join Date: Jun 2010
Location: Italy
Posts: 100
Rep Power: 15 |
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. |
|
September 14, 2012, 11:15 |
|
#8 |
Senior Member
KHB
Join Date: Aug 2010
Location: Singapore
Posts: 118
Rep Power: 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?
|
|
September 17, 2012, 03:03 |
|
#9 |
New Member
Jan Willem Krijger
Join Date: May 2010
Posts: 8
Rep Power: 15 |
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. |
|
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
Difficulty in calculating angular velocity of Savonius turbine simulation | alfaruk | CFX | 14 | March 17, 2017 06:08 |
Velocity profile disturbance due to loss coefficient | rks171 | Main CFD Forum | 3 | May 25, 2012 17:30 |
Numerical wave tank | Bridget | FLUENT | 0 | March 27, 2006 16:09 |
Numerical Method | Andrew Hayes | Main CFD Forum | 5 | June 17, 2005 09:17 |
Convection velocity of Coherent structures | Jongdae Kim | Main CFD Forum | 3 | February 5, 2002 04:04 |