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

Traction boundary conditions

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

Reply
 
LinkBack Thread Tools Display Modes
Old   January 11, 2004, 11:04
Default Traction boundary conditions
  #1
m malik
Guest
 
Posts: n/a
I have the following question on 3-dimensional FEM solution of momentum-continuity equations. Consider a simple capillary flow problem with only the pressure being specified at the two ends; velocities not specified. How does one apply the traction conditions: ,i,e, tx = (mu)(du/dz+dw/dx), ty = (mu)(dv/dz+dw/dy), and tz = -p+2(mu)(dw/dz) when velocity field is not know a-priori? (z = coordinate along the capillary axis). Thanks.
  Reply With Quote

Old   January 12, 2004, 19:40
Default Re: Traction boundary conditions
  #2
xueying
Guest
 
Posts: n/a
The traction equals t = -p n + mu n.(du/dx + transpose(du/dx)) where t, n, u, x are vectors

In my code, I specify the traction as follows, If the flow is fully developed, then n.(du/dx)=0, so t = -p n + mu n.(transpose(du/dx)) The traction is encoded thru the weak form integral, du/dx is computed from the finite element basis functions and coefficients.

You can also refer to papers related with open flow boundaries.
  Reply With Quote

Old   January 13, 2004, 09:37
Default Re: Traction boundary conditions
  #3
m malik
Guest
 
Posts: n/a
I am dealing with the polymer flows, and in my code I apply the traction boundary condition in the following manner. The nonlinear finite element equations are solved using the Picard iteration scheme. In each iteration, the traction vector is calculated using the external pressure and the mu.(dui/dxj + duj/dxi) terms from the velocity field of the previous iteration. No assumption of fully developed flow is imposed. Is this the right approach?
  Reply With Quote

Old   January 13, 2004, 12:56
Default Re: Traction boundary conditions
  #4
xueying
Guest
 
Posts: n/a
If it's not fully developed flow and it's a viscous flow, your imposing method should be correct, at least we impose exactly the same traction.

Since your flow is polymer flow, do you have elastic stress contribution from polymer? In our code, if it's polymer flow, then it's viscoelastic flow, the traction has contributions from pressure, viscous stress, and elastic stress.
  Reply With Quote

Old   January 13, 2004, 13:49
Default Re: Traction boundary conditions
  #5
m malik
Guest
 
Posts: n/a
Thanks Xueying for your response. No, I do not have elastic stress contribution. You are probably talking about the elastic dumbbell models. I am just considering steady state viscoplatic flows. However, irrespective of the model, why should one impose fully developed flow condition? For example in tube flow, the solution must approach to fully developed with increasing aspect (length-to-diameter) ratio. (This is one of the things that is bothering me.)
  Reply With Quote

Old   January 14, 2004, 05:15
Default Re: Traction boundary conditions
  #6
Rami
Guest
 
Posts: n/a
<html>

<head> <meta http-equiv=Content-Type content="text/html; charset=windows-1255"> <meta name=Generator content="Microsoft Word 10 (filtered)"> <title>Re: Traction boundary conditions</title>

<style>

</style>

</head>

<body lang=EN-US>

<div class=Section1>

<p class=MsoNormal style='text-align:justify;text-indent:.2in'>I think a formal and general answer would be the simplest way to answer your question. Tensor notation is used below, in which a repeated index implies summation. In addition, "," stands for covariant derivative (which, for Cartesian coordinates, degenerates to partial derivative).


<p class=MsoNormal style='text-align:justify;text-indent:.2in'>The traction vector, t<sub>k</sub>, in a given direction n<sub>i</sub> is defined as


<p class=MsoNormal style='margin-left:.5in;text-align:justify;text-indent:.2in'>t<sub>k</sub> = <span style='font-family:Symbol'>s</span><sub>ik</sub> n<sub>i</sub>


<p class=MsoNormal style='text-align:justify'>where <span style='font-family: Symbol'>s</span><sub>ik</sub> is the stress tensor.


<p class=MsoNormal style='text-align:justify;text-indent:.2in'>The constitutive relation for a fluid with no elasticity is


<p class=MsoNormal style='margin-left:.5in;text-align:justify;text-indent:.2in'><span style='font-family:Symbol'>s</span><sub>ik</sub> = -p <span style='font-family:Symbol'>d</span><sub>ik</sub> + <span style='font-family: Symbol'>m</span><sub>v</sub> <span style='font-family:Symbol'>d</span><sub>ik</sub> <span style='font-family:Symbol'>e</span><sub>mm</sub> + 2<span style='font-family:Symbol'>m</span> (<span style='font-family:Symbol'>e</span><sub>ik</sub> 1/3 <span style='font-family:Symbol'>d</span><sub>ik</sub> <span style='font-family:Symbol'>e</span><sub>mm</sub>)


<p class=MsoNormal style='text-align:justify'>where p is the pressure, <span style='font-family:Symbol'>m</span> and <span style='font-family:Symbol'>m</span><sub>v</sub> are the viscosity and the bulk viscosity, respectively, <span style='font-family:Symbol'>d</span><sub>ik</sub> is Kronecker's delta and the strain-rate tensor, <span style='font-family:Symbol'>e</span><sub>ik</sub> , is related to the velocity vector, u<sub>k</sub>, by


<p class=MsoNormal style='margin-left:.5in;text-align:justify;text-indent:.2in'><span style='font-family:Symbol'>e</span><sub>ik</sub> = 1/2 (u<sub>i,k</sub> + u<sub>k</sub><sub>,i</sub>)


<p class=MsoNormal style='text-align:justify;text-indent:.2in'>In the finite element method, the shape-functions relate the nodal values to the element distributions. Therefore, having the nodal values (at any iteration level), the traction may be calculated by the above equations.


<p class=MsoNormal style='text-align:justify;text-indent:.2in'>A developed flow assumption is not required in a pipe flow. You may definitely solve for a developing flow. For a long enough domain you will notice the flow approaches the fully developed profile asymptotically.


<p class=MsoNormal align=center style='text-align:center;text-indent:.2in'>I hope this helps,


<p class=MsoNormal align=center style='text-align:center;text-indent:.2in'>Rami


</div>

</body>

</html>
  Reply With Quote

Old   March 29, 2012, 12:46
Default
  #7
Member
 
Hesam Moghaddam
Join Date: Mar 2012
Posts: 49
Rep Power: 5
hesamking is on a distinguished road
Hi,
How can I apply free traction BC in CFX?
my BC is:
du/dn=0
thank you so much
Hesam
hesamking 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
Boundary conditions for 2D Navie-Stockes simulation L1011 OpenFOAM 5 December 13, 2012 09:17
Impinging Jet Boundary Conditions Anindya Main CFD Forum 24 January 11, 2012 14:40
Concentric tube heat exchanger (Air-Water) Young CFX 5 October 6, 2008 23:17
Trimmed cell and embedded refinement mesh conversion issues michele OpenFOAM Other Meshers: ICEM, Star, Ansys, Pointwise, GridPro, Ansa, ... 2 July 15, 2005 04:15
A problem about setting boundary conditions lyang Main CFD Forum 0 September 19, 1999 18:29


All times are GMT -4. The time now is 22:48.