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

[HELP] Slip flow boundary condtion in CFX

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

Reply
 
LinkBack Thread Tools Display Modes
Old   March 3, 2010, 16:01
Default [HELP] Slip flow boundary condtion in CFX
  #1
New Member
 
Mengbai Wu
Join Date: Mar 2010
Posts: 7
Rep Power: 7
jeffwmb is on a distinguished road
Hey friends:

I am dealing with this gas flow field calculation in CFX. I have a relatively large Knudsen number, which is about 0.03. In this range NS equations still work but the no-slip boundary condition needs to be revised accoding to either the first order or the second order slip velocity condition. I am not sure whether CFX can handle this problem. I am new to CFX.

Thanks for any possible help.
jeffwmb is offline   Reply With Quote

Old   March 3, 2010, 17:57
Default
  #2
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,672
Rep Power: 84
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
You will need to define a wall shear stress to do this. Hopefully you can do this using CEL.
ghorrocks is offline   Reply With Quote

Old   March 3, 2010, 18:47
Default
  #3
New Member
 
Mengbai Wu
Join Date: Mar 2010
Posts: 7
Rep Power: 7
jeffwmb is on a distinguished road
Thanks very much.

I am using ANSYS CFX 11.0. I don't think it can define wall shear stress directly. I just saw a ANSYS 12.1 technical specification note, which showed that ANAYS 12.1 can do finite slip and wall specified shear stress.
CEL is a good idea, I am thinking about do a user subroutine now.

Thank you again.
jeffwmb is offline   Reply With Quote

Old   June 8, 2011, 03:26
Default
  #4
New Member
 
siva
Join Date: Sep 2009
Posts: 7
Rep Power: 7
ch05d007 is on a distinguished road
hai

I too have the same problem. i can see some documentation in ansys 12 where wall shear stress components can be given but this option is not available in ansys 11.


have u identify this option in ansys 12.
ch05d007 is offline   Reply With Quote

Old   September 14, 2012, 06:14
Default
  #5
New Member
 
Ramin Mirzazadeh
Join Date: Aug 2012
Posts: 16
Rep Power: 4
raminmir is on a distinguished road
Hello
Having a knudsen number around 0.01, I tried to do a laminar flow analysis in a simple rectangular micro duct, I used CEL for introducing the first order slip boundary model through specified shear stress on walls. I got consistent results comparing with analytical solution for steady state analysis, which shows the CEL is physically right, when I do the same analysis but in transient approach, cfx gives error "Floating point exception: Overflow".
I read http://www.cfd-online.com/Wiki/Ansys...publishable.3F, and I tried all of its suggestions (mesh change, time step change,short intial time steps,upwind option, no. of coef. loops change )but does not work.
can anyone give any hint on it? is there any problem in CFX for transient analysis of slip boundary?
Thanks in advance
raminmir is offline   Reply With Quote

Old   September 14, 2012, 07:48
Default
  #6
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,672
Rep Power: 84
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
First of all I would run your simulation with normal no slip boundaries. That makes sure your general setup is OK.
ghorrocks is offline   Reply With Quote

Old   September 14, 2012, 09:29
Default
  #7
New Member
 
Ramin Mirzazadeh
Join Date: Aug 2012
Posts: 16
Rep Power: 4
raminmir is on a distinguished road
exactly, I did that already. as soon as I use the CEL code that in steady state works, CFX cant handle anymore
raminmir is offline   Reply With Quote

Old   September 14, 2012, 09:39
Default
  #8
New Member
 
Ramin Mirzazadeh
Join Date: Aug 2012
Posts: 16
Rep Power: 4
raminmir is on a distinguished road
for further information, I used the following CEL


ShearSlipU = -ave(Velocity u)@wall1*1.8E-5[N s m^-2]/(1.2222*MeanFreePath)
MeanFreePath = boltzmann*298[K]/(sqrt(2)*pi*ave(Absolute Pressure )@REGION:B16*MolecularDiam^2)
MolecularDiam = 3.7e-10[m]

1.8e-5 is viscosity and 1.2222 is a constant related to tangential momentum accommodation coefficient.
raminmir is offline   Reply With Quote

Old   September 14, 2012, 10:27
Default
  #9
Senior Member
 
Lance
Join Date: Mar 2009
Posts: 522
Rep Power: 11
Lance is on a distinguished road
Wouldnt ShearSlipU become an extremely small number? like 1e-17 or so? What do you estimate it to be?
Lance is offline   Reply With Quote

Old   September 14, 2012, 10:54
Default
  #10
New Member
 
Ramin Mirzazadeh
Join Date: Aug 2012
Posts: 16
Rep Power: 4
raminmir is on a distinguished road
ciao Lance,
shear stress at wall, in CFX for steady state analysis yields to 0.2499 Pa and analytically it should be 0.226 Pa
raminmir is offline   Reply With Quote

Old   September 14, 2012, 11:00
Default
  #11
Senior Member
 
Lance
Join Date: Mar 2009
Posts: 522
Rep Power: 11
Lance is on a distinguished road
I see. Well, one reason to the overflow could be that during the startup of your simulation one of the variables (U or abs pressure) fluctuate a bit and causes your expression to overflow.
Lance is offline   Reply With Quote

Old   September 14, 2012, 11:08
Default
  #12
New Member
 
Ramin Mirzazadeh
Join Date: Aug 2012
Posts: 16
Rep Power: 4
raminmir is on a distinguished road
I had set initialisation values to Zero, it might be the reason for overflow, I will do analysis with U value half of expected steady state value which is 0.6225 m/s. can this help analysis to converge?

thanks for you idea
raminmir is offline   Reply With Quote

Old   September 15, 2012, 07:12
Default
  #13
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,672
Rep Power: 84
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
If you are still having convergence difficulties then I suspect the issue will be the way you are coupling the velocity at the control volume adjacent to the wall to the wall shear stress. This, in effect, sets up a new numerical relationship which needs solution. As the ave() function is evaluated based on the variabel values from the last iteration, this means you are in effect doing an explicit calculation of the the wall condition and this means your allowable time step size will be massively reduced or the simulation goes unstable and diverges.

If this is correct then the fix is simple - a smaller time step size. And the required time step might be massively smaller than you currently run - like 1000 times smaller, not half.
ghorrocks is offline   Reply With Quote

Old   September 15, 2012, 07:17
Default
  #14
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,672
Rep Power: 84
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
Also, why do you use an average function anyway? If you define ShearSlipU = -Velocity u*1.8E-5[N s m^-2]/(1.2222*MeanFreePath) then the function can vary over the wall, which sounds more correct to me.
ghorrocks is offline   Reply With Quote

Old   September 18, 2012, 10:14
Default
  #15
New Member
 
Ramin Mirzazadeh
Join Date: Aug 2012
Posts: 16
Rep Power: 4
raminmir is on a distinguished road
changing the initialisation values did not help.
thanks Glenn for the idea, I tried sensitivity analysis and the problem converged. I used 1e-7 s timsteps, also I used tight RMS residual target 1e-10 with max coeff. loop of 100. I am not professional with CFX and I read cfx manual and this forum to get information about RMS residual target and coeff loops. cfx manual suggests RMS 1e-5 and up to 10 loops for most of problems but still not sure what this value should be for Microscale problems or the importance of coeff loops. it would be helpful if you can give some hints about them. Thanks
raminmir is offline   Reply With Quote

Old   September 18, 2012, 19:38
Default
  #16
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,672
Rep Power: 84
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
The documentation's guide is good for most classes of flow. As long as your Re>0.01 or so you should be fine. And for single phase flows you should probably aim for 3-5 coeff loops for time step, 10 is a bit too many.
ghorrocks is offline   Reply With Quote

Old   March 13, 2013, 11:14
Default
  #17
New Member
 
kullimanali
Join Date: Dec 2012
Posts: 13
Rep Power: 4
arunbaghel is on a distinguished road
Quote:
Originally Posted by ghorrocks View Post
You will need to define a wall shear stress to do this. Hopefully you can do this using CEL.
I am doing same thing using ansys fluent, can u give some steps for calculating wall shear stress using cel
arunbaghel is offline   Reply With Quote

Old   March 13, 2013, 11:17
Default
  #18
Senior Member
 
Lance
Join Date: Mar 2009
Posts: 522
Rep Power: 11
Lance is on a distinguished road
1) why not try the fluent forum?
2) CEL is not available in fluent
3) you dont calculate wall shear stress with CEL
Lance is offline   Reply With Quote

Old   March 13, 2013, 11:17
Default
  #19
New Member
 
kullimanali
Join Date: Dec 2012
Posts: 13
Rep Power: 4
arunbaghel is on a distinguished road
Quote:
Originally Posted by jeffwmb View Post
Hey friends:

I am dealing with this gas flow field calculation in CFX. I have a relatively large Knudsen number, which is about 0.03. In this range NS equations still work but the no-slip boundary condition needs to be revised accoding to either the first order or the second order slip velocity condition. I am not sure whether CFX can handle this problem. I am new to CFX.

Thanks for any possible help.
hi,
i am doing same thing,can you explain if u got solution, how to calculate shear stress at wall
arunbaghel is offline   Reply With Quote

Old   March 13, 2013, 11:38
Default
  #20
New Member
 
kullimanali
Join Date: Dec 2012
Posts: 13
Rep Power: 4
arunbaghel is on a distinguished road
Quote:
Originally Posted by Lance View Post
1) why not try the fluent forum?
2) CEL is not available in fluent
3) you dont calculate wall shear stress with CEL
hi, please help me could u give some steps for this
shear stress calculation in ansys fluent
arunbaghel is offline   Reply With Quote

Reply

Tags
slip flow

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
3-D Compressible Flow Boundary Conditions Tyler FLUENT 4 February 5, 2009 20:58
Mass flow and U-Mom flow in CFX Zhihua Xie CFX 0 September 3, 2007 09:49
Flow Direction: normal to boundary!!! Atit CFX 0 June 26, 2007 06:48
Slip boundary condition what is inside normunds OpenFOAM Running, Solving & CFD 2 June 4, 2007 06:45
maintaining a logarithmic velocity distribution Morten Andersen CFX 1 January 8, 2007 12:37


All times are GMT -4. The time now is 03:59.