[HELP] Slip flow boundary condtion in CFX
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 noslip 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. 
You will need to define a wall shear stress to do this. Hopefully you can do this using CEL.

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. 
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. 
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.cfdonline.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 
First of all I would run your simulation with normal no slip boundaries. That makes sure your general setup is OK.

exactly, I did that already. as soon as I use the CEL code that in steady state works, CFX cant handle anymore

for further information, I used the following CEL
ShearSlipU = ave(Velocity u)@wall1*1.8E5[N s m^2]/(1.2222*MeanFreePath) MeanFreePath = boltzmann*298[K]/(sqrt(2)*pi*ave(Absolute Pressure )@REGION:B16*MolecularDiam^2) MolecularDiam = 3.7e10[m] 1.8e5 is viscosity and 1.2222 is a constant related to tangential momentum accommodation coefficient. 
Wouldnt ShearSlipU become an extremely small number? like 1e17 or so? What do you estimate it to be?

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 
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.

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 
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. 
Also, why do you use an average function anyway? If you define ShearSlipU = Velocity u*1.8E5[N s m^2]/(1.2222*MeanFreePath) then the function can vary over the wall, which sounds more correct to me.

changing the initialisation values did not help.
thanks Glenn for the idea, I tried sensitivity analysis and the problem converged. I used 1e7 s timsteps, also I used tight RMS residual target 1e10 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 1e5 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 
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 35 coeff loops for time step, 10 is a bit too many.

Quote:

1) why not try the fluent forum?
2) CEL is not available in fluent 3) you dont calculate wall shear stress with CEL 
Quote:
i am doing same thing,can you explain if u got solution, how to calculate shear stress at wall 
Quote:
shear stress calculation in ansys fluent 
All times are GMT 4. The time now is 04:32. 