CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Main CFD Forum

NAvier Stokes and Newton's law coupling

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

Like Tree3Likes
  • 1 Post By duri
  • 1 Post By duri
  • 1 Post By leflix

Reply
 
LinkBack Thread Tools Display Modes
Old   May 28, 2013, 21:59
Default NAvier Stokes and Newton's law coupling
  #1
Member
 
sud
Join Date: May 2013
Posts: 65
Rep Power: 4
archeoptyrx is on a distinguished road
Hello ppl ,

I am trying to simulate the Navier Stokes Equation for a body falling which starts with some velocity at an altitude .

The velocity is not a constant one . It is going to vary for each time step and the height as per newton's law.

I wrote code for numerically simulating the NS Equation neglecting body forces .

Now i incorporate the body force (rho*g) into it .

I need to couple the navier stokes and newton's law together . How do i implement it ?

Any suggestions will be of great help . And i m desperately searching things to compete my project .

Thanks
archeoptyrx is offline   Reply With Quote

Old   June 3, 2013, 08:50
Default
  #2
Senior Member
 
duri
Join Date: May 2010
Posts: 130
Rep Power: 7
duri is on a distinguished road
You cannot couple body motion to NS equations because, NS is for flow field. If you add body force to equation it works on fluid and not on the body. You can do it by two ways,
1. Find distance time relation for the body and apply grid motion in unstready flow field. If you are writing your own code, need to correct flux calculations based on wall motion.
2. Find velocity time relation for the body and apply it as inlet condtion. Time varying inlet boundary condition.

Thanks
archeoptyrx likes this.
duri is offline   Reply With Quote

Old   June 3, 2013, 14:24
Default
  #3
Member
 
Jonas T. Holdeman, Jr.
Join Date: Mar 2009
Location: Knoxville, Tennessee
Posts: 94
Rep Power: 9
Jonas Holdeman is on a distinguished road
I would expect that you would be working in an accelerating coordinate system where the falling object is stationary. The fluid would be accelerating at rate g minus the result of the drag force. As you say, the fluid would be subject to a body force (rho*g) minus the drag force which you would calculate at each time step from the flow. As the fluid velocity increases the drag force increases until the drag balances the gravitational force. The velocity at which these balance is called the terminal velocity.
Jonas Holdeman is offline   Reply With Quote

Old   June 4, 2013, 12:32
Default
  #4
Member
 
sud
Join Date: May 2013
Posts: 65
Rep Power: 4
archeoptyrx is on a distinguished road
Thanks Mr. duri . I wrote a code for complete navier stokes equation in viscous supersonic flow long back . Now i wish to simulate the code for any body which is at an altitude of 60km and starts with supersonic velocity and then it gradually drops to zero when it reaches the ground .

I need to extend this navier stokes code to produce the pressure plots throughout the atmosphere as it starts from 60km till ground . you said me to use time dependent boundary condition . But i haven't used it in any of my simulation and i really wanted to do this project.

Can you help me out ?
archeoptyrx is offline   Reply With Quote

Old   June 4, 2013, 12:35
Default
  #5
Member
 
sud
Join Date: May 2013
Posts: 65
Rep Power: 4
archeoptyrx is on a distinguished road
Quote:
Originally Posted by Jonas Holdeman View Post
I would expect that you would be working in an accelerating coordinate system where the falling object is stationary. The fluid would be accelerating at rate g minus the result of the drag force. As you say, the fluid would be subject to a body force (rho*g) minus the drag force which you would calculate at each time step from the flow. As the fluid velocity increases the drag force increases until the drag balances the gravitational force. The velocity at which these balance is called the terminal velocity.
Jonas T. Holdeman, Jr.

I understand what you said . The thing i wanted to do is just to simulate the navier stokes code at all points in the atmosphere coupled with reentry dynamics of the body .
how could I proceed ? ..
archeoptyrx is offline   Reply With Quote

Old   June 18, 2013, 04:18
Default
  #6
Senior Member
 
duri
Join Date: May 2010
Posts: 130
Rep Power: 7
duri is on a distinguished road
The easiest way to implement is to use your unsteady code (dual time stepping method is better). Converge solution for initial condition, then solve at minimum one DOF equation and estimate new velocity of body (time integration) and estimate new bc condition.
If you are comfortable with LODI BC's then use them for unsteady BC.
archeoptyrx likes this.
duri is offline   Reply With Quote

Old   September 6, 2013, 09:46
Default
  #7
Member
 
sud
Join Date: May 2013
Posts: 65
Rep Power: 4
archeoptyrx is on a distinguished road
Quote:
Originally Posted by duri View Post
The easiest way to implement is to use your unsteady code (dual time stepping method is better). Converge solution for initial condition, then solve at minimum one DOF equation and estimate new velocity of body (time integration) and estimate new bc condition.
If you are comfortable with LODI BC's then use them for unsteady BC.
Ok . Lets take a simple problem . A solid body falling down due to gravity into a viscous fluid . It undergoes tumbling. How do i numerically simulate the problem? what equations should be used to simulate the problem ? . My professor said about the mass ratio which is gonna influence the problem .
archeoptyrx is offline   Reply With Quote

Old   September 7, 2013, 01:46
Default
  #8
Senior Member
 
duri
Join Date: May 2010
Posts: 130
Rep Power: 7
duri is on a distinguished road
I think probably you are talking about multiphase VOF. Its better to try this problem in fluent (probably cfx). It has both vof model and 6dof model and quite easy to setup the solution.
duri is offline   Reply With Quote

Old   September 15, 2013, 15:26
Wink
  #9
Senior Member
 
Join Date: Aug 2011
Posts: 251
Rep Power: 7
leflix is on a distinguished road
Quote:
Originally Posted by duri View Post
You cannot couple body motion to NS equations because, NS is for flow field. If you add body force to equation it works on fluid and not on the body.

Of course you can !!!!

first of all it depends on the size of your object relatively to the size of your mesh cells.
first option: your object has a smaller size thant your grid size.
1) solve your navier-stokes equations accounting for retro-acting force (Two way coupling)
2) compute the fluid forces acting on your solid (drag,lift, magnun safftman forces etc.....) these forces depend on the fluid velocity U.
3) solve newton's law mdV/dt = Summ of all forces (V is the velocity of your object)
4) solve dx/dt=V then you get the new position of your object
5)compute the retro-acting force depending on the location of your object which act as source term in Navier-Stokes equation. This retro-acting force may be -(summ of all forces) you computed in the newton's law

second option your object is much greater that your grid size.
I would suggest the use of an Immersed Boundary Method. These kind of methods help the fluid to feel the presence of the obstacle. Many options are available. The newton 's law will tell where the object is in the domain at every time step.
Now the forces acting on the object will be computed from the integral over the surface of the object of sigma.n.ds where sigma is the stress tensor = -P II + Tau where P is the pressure, II Identity tensor and Tau viscous stress tensor. This can be computed once velocity and pressure are known.
Godd luck
archeoptyrx likes this.
leflix is offline   Reply With Quote

Old   September 30, 2013, 16:13
Red face
  #10
Member
 
sud
Join Date: May 2013
Posts: 65
Rep Power: 4
archeoptyrx is on a distinguished road
Quote:
Originally Posted by leflix View Post
Of course you can !!!!

first of all it depends on the size of your object relatively to the size of your mesh cells.
first option: your object has a smaller size thant your grid size.
1) solve your navier-stokes equations accounting for retro-acting force (Two way coupling)
2) compute the fluid forces acting on your solid (drag,lift, magnun safftman forces etc.....) these forces depend on the fluid velocity U.
3) solve newton's law mdV/dt = Summ of all forces (V is the velocity of your object)
4) solve dx/dt=V then you get the new position of your object
5)compute the retro-acting force depending on the location of your object which act as source term in Navier-Stokes equation. This retro-acting force may be -(summ of all forces) you computed in the newton's law

second option your object is much greater that your grid size.
I would suggest the use of an Immersed Boundary Method. These kind of methods help the fluid to feel the presence of the obstacle. Many options are available. The newton 's law will tell where the object is in the domain at every time step.
Now the forces acting on the object will be computed from the integral over the surface of the object of sigma.n.ds where sigma is the stress tensor = -P II + Tau where P is the pressure, II Identity tensor and Tau viscous stress tensor. This can be computed once velocity and pressure are known.
Godd luck
Very great information Mr. leflix . It will be good if further advice regarding the problem is specified . My domain is a rectangle with the plate wall to the bottom(right-inlet, left-outlet,top-freestream). Now the stability criteria for the explicti numerical method suggests me to use delta t = 1e-5 for CFD numerical simulation. At time t =0, U=1000m/s , delta t =1e-5, after one time step, i find the pressure distribution , temperature distribution and all other properties on the plate wall . Now, i have two questions ,
  1. u asked me to find the retro acting forces . How do i find it ? i just got the distribution.
  2. If i find those retro acting forces and use in equations of motion, with the same delta t =1e-5 and solve for V(t), gives me V after delta t seconds . What should i do now ? should I use the new V(delta t) as initial condition, and the pressure ,temperature at each grid point for the next time step?? and solve for the new flow properties at each grid point for second time step and so on ??


Thanks in advance ..
archeoptyrx is offline   Reply With Quote

Old   March 6, 2014, 03:42
Default Navier stokes streamline vorticity approach
  #11
New Member
 
Rajashekaran
Join Date: Mar 2014
Posts: 2
Rep Power: 0
raja.shekaran2000 is on a distinguished road
Can anyone having the solved example of Streamline Vorticity approach and Navier stoke equation to find the pressure velocity Ux and Uy in 2D.
I found in book only the derivation but i need the solved example for finding pressure and velocity by discritizing and iterative method.

Regards
K.Rajashekaran
raja.shekaran2000 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



All times are GMT -4. The time now is 22:43.