CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > STAR-CCM+

Numerical Towing Tank Velocity Ramp

Register Blogs Members List Search Today's Posts Mark Forums Read

Reply
 
LinkBack Thread Tools Display Modes
Old   July 30, 2012, 23:52
Default Numerical Towing Tank Velocity Ramp
  #1
Senior Member
 
KHB
Join Date: Aug 2010
Location: Singapore
Posts: 107
Rep Power: 6
lava12005 is on a distinguished road
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?
lava12005 is offline   Reply With Quote

Old   July 31, 2012, 03:17
Default
  #2
Member
 
sanjay's Avatar
 
aerosapien
Join Date: Sep 2010
Posts: 59
Rep Power: 6
sanjay is on a distinguished road
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
sanjay is offline   Reply With Quote

Old   July 31, 2012, 03:29
Default
  #3
Senior Member
 
KHB
Join Date: Aug 2010
Location: Singapore
Posts: 107
Rep Power: 6
lava12005 is on a distinguished road
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?
lava12005 is offline   Reply With Quote

Old   July 31, 2012, 04:12
Default
  #4
New Member
 
Jan Willem Krijger
Join Date: May 2010
Posts: 6
Rep Power: 7
Sideshore is on a distinguished road
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!
Sideshore is offline   Reply With Quote

Old   July 31, 2012, 09:27
Default
  #5
Member
 
Ryan Coe
Join Date: Jun 2010
Location: Albuquerque, NM
Posts: 98
Rep Power: 7
ryancoe is on a distinguished road
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
ryancoe is offline   Reply With Quote

Old   August 17, 2012, 00:27
Default
  #6
Senior Member
 
KHB
Join Date: Aug 2010
Location: Singapore
Posts: 107
Rep Power: 6
lava12005 is on a distinguished road
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).
lava12005 is offline   Reply With Quote

Old   September 5, 2012, 06:13
Default
  #7
Senior Member
 
Henry Arrigo
Join Date: Jun 2010
Location: Italy
Posts: 100
Rep Power: 7
Henry Arrigo is on a distinguished road
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.
Henry Arrigo is offline   Reply With Quote

Old   September 14, 2012, 11:15
Default
  #8
Senior Member
 
KHB
Join Date: Aug 2010
Location: Singapore
Posts: 107
Rep Power: 6
lava12005 is on a distinguished road
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?
lava12005 is offline   Reply With Quote

Old   September 17, 2012, 03:03
Default
  #9
New Member
 
Jan Willem Krijger
Join Date: May 2010
Posts: 6
Rep Power: 7
Sideshore is on a distinguished road
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.
Sideshore is offline   Reply With Quote

Reply

Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Difficulty in calculating angular velocity of Savonius turbine simulation alfaruk CFX 8 December 3, 2013 17:51
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 05:04


All times are GMT -4. The time now is 01:17.