
[Sponsors] 
December 10, 2012, 14:56 
UDF for slip boundary condition

#1 
New Member
rasoul b
Join Date: Dec 2010
Location: iran
Posts: 13
Rep Power: 15 
Hi all
I have written a UDF for slip boundary condition (=*du_dy) by C_U_G(c,t)[1] Macro. 1 I test my UDF for 2 & 3D steady laminar channel flow, it's work good with low slip length (0.00010.005) but for larger slip length not converged. Can anyone guide me for this convergence problem? 2. I need to use velocity gradient of previous time step for unsteady simulation. what macros I should use? thanks 

December 10, 2012, 15:13 

#2 
Super Moderator
Alex
Join Date: Jun 2012
Location: Germany
Posts: 3,384
Rep Power: 46 
Do you know that a boundary condition like this is already implemented in Fluent?


December 10, 2012, 15:29 

#3 
New Member
rasoul b
Join Date: Dec 2010
Location: iran
Posts: 13
Rep Power: 15 
what version? please guide me
Thanks 

December 10, 2012, 17:42 

#4 
Super Moderator
Alex
Join Date: Jun 2012
Location: Germany
Posts: 3,384
Rep Power: 46 
Last time i read about it was in the version 13 manual, but i think it can also be found in earlier versions.
I am out of office right now, so all I can do is recommend a google search with 'fluent high knudsen boundary'. I think you will figure it out by yourself, otherwise feel free ask again. 

December 11, 2012, 03:46 

#5 
New Member
rasoul b
Join Date: Dec 2010
Location: iran
Posts: 13
Rep Power: 15 
slip velocity based on knudsen number is appropriate for gases and Not applicable for liquids. please say another method.
thanks 

December 11, 2012, 05:07 

#6 
Super Moderator
Alex
Join Date: Jun 2012
Location: Germany
Posts: 3,384
Rep Power: 46 
This holds true for a microscopic point of view.
But if you just want a boundary condition in the form (=*du_dy), the high Knudsen number boundary condition in fluent is the right choice, no matter what type of fluid you are using. 

December 13, 2012, 12:56 

#7 
New Member
rasoul b
Join Date: Dec 2010
Location: iran
Posts: 13
Rep Power: 15 
thanks flotus1 for your answers.
high Knudsen number boundary condition is for LowPressure Gas Systems and available only when the Laminar model is selected in the Viscous Model panel (based on explanation expressed in fluent 6.3 help). but my Model is LES and pressure is high in my case. 

December 14, 2012, 05:53 

#8 
Super Moderator
Alex
Join Date: Jun 2012
Location: Germany
Posts: 3,384
Rep Power: 46 
"high" pressure is not the problem in your case.
The boundary treatment can be used at any pressure level. The term "low pressure" comes from one of the applications of the model in lowpressure systems. But the model is appropriate at arbitrary pressure levels, whenever the Knudsen number is high. I am currently studying flows at normal pressure levels with a BC like this. But I see now that this BC is not an option since your Model is LES. Perhaps it is possible to activate the BC with a LES model with a text command. This would be a question for the fluent support. 

November 13, 2014, 05:03 
hi

#9 
Member
Qureshi M Z I
Join Date: Sep 2013
Posts: 79
Rep Power: 12 
hi, i need a UDF for slip boundary condition at the bottom of the domain or at the ground (wall), case is just like a flow over a building. if anybody have sample UDF please share this, z is a vertical axis of my domain. thanks
mziqureshi@hotmail.com regards, 

November 13, 2014, 05:12 

#10  
Senior Member
Join Date: Nov 2013
Posts: 1,965
Rep Power: 26 
Quote:


November 13, 2014, 09:42 

#11 
Member
Qureshi M Z I
Join Date: Sep 2013
Posts: 79
Rep Power: 12 
hi, thanks pakk, here rasoulb use slip length instead of dynamic viscosity, as given in the link
http://www.cfdonline.com/Wiki/Wall_shear_stress do u know the relationship between slip length and dynamic viscosity. thanks 

November 13, 2014, 10:13 

#12 
Senior Member
Join Date: Nov 2013
Posts: 1,965
Rep Power: 26 
First question you should ask yourself: What is the equation for slip that you want to implement?
Second question you should ask yourself: What is the equation for slip that Fluent has implemented? (This is written in the Help, look it up.) Third question: How can you choose parameters such that the Fluent implementation is the same as what you want? 

March 20, 2019, 11:37 
UDF for slip boundary condition

#13 
New Member
Join Date: Feb 2016
Posts: 20
Rep Power: 10 
Here is a code for applying a wall slip velocity based on wall slip layer thickness and the strain rate (which corresponds to ) at the wall.
To make it work, some underrelaxation is required for the calculated tangential wall velocity . BTW: The formula for Maxwellbased Slip Boundary Formulation for LowPressure Gas Systems (https://www.sharcnet.ca/Software/Flu...ug/node613.htm) is not applicable for cases, where there is a significant pressure and/or temperature change within the domain, since the parameter is autocalculated by fluent. Hence, it is not possible to set and in way to get a constant factor left of the term , which is an approximation for . Now, here is the code: Code:
#include "udf.h" /* =============================================== Velocity slip at wall boundaries separate routines for every velocity coordinate UDF can be interpreted at least 2 userdefined memories (UDM) need to be allocated first! =============================================== */ // wall slip layer thickness [m] #define DELTA 10.0e6 // underrelaxation factor for tangential wall velocity #define RELAX_CT 0.1 DEFINE_PROFILE(slip_velocity_x,f_thread,index) { face_t face; cell_t cell; Thread *c_thread; real u, v; real ct, cx; real gamma; int i; begin_f_loop(face,f_thread) // for each face: get faceid and thread { cell=F_C0(face,f_thread); // get corresponding cell c_thread=THREAD_T0(f_thread); // get cell thread u = C_U(cell,c_thread); // F_U(face,f_thread); // get cell center velocity u v = C_V(cell,c_thread); // F_V(face,f_thread); // get cell center velocity v gamma = C_STRAIN_RATE_MAG(cell,c_thread); // get strain rate (equivalent to du/dn at wall) ct = (1RELAX_CT)*F_UDMI(face,f_thread,0)+RELAX_CT*DELTA*gamma; // calculate tangential velocity (with underrelaxation using previous calculation step) F_UDMI(face,f_thread,0)=ct; //store in userdefined face memory (id=0) for next calculation cx = ct*u/sqrt(u*u+v*v); // component of ct in xdirection F_PROFILE(face,f_thread,index) = cx; // assign to profile } end_f_loop(face,f_thread) } DEFINE_PROFILE(slip_velocity_y,f_thread,index) { face_t face; cell_t cell; Thread *c_thread; real u, v; real ct, cy; real gamma; begin_f_loop(face,f_thread) { cell=F_C0(face,f_thread); // get cell c_thread=THREAD_T0(f_thread); // get cell thread u = C_U(cell,c_thread); // F_U(face,f_thread); v = C_V(cell,c_thread); // F_V(face,f_thread); gamma = C_STRAIN_RATE_MAG(cell,c_thread); ct = (1RELAX_CT)*F_UDMI(face,f_thread,1)+RELAX_CT*DELTA*gamma; F_UDMI(face,f_thread,1)=ct; cy = ct*v/sqrt(u*u+v*v); F_PROFILE(face,f_thread,index) = cy; } end_f_loop(face,f_thread) } 

May 3, 2020, 13:58 
UDF for slip velocity and temperature jump

#14 
Member
Homayoon sohrabi
Join Date: May 2020
Posts: 56
Rep Power: 5 
Hello everyone
I'm having problem with writing UDF for these two functions(slip velocity and temperature jump) below for a liquidsolid interface: 1. V= L(du/dy) 2. T)f = T)s + L(dT/dy) in which V is slip velocity, u is mean velocity along with x axis, T)f is fluid temperature and T)s is solid temperature I would appreciate very much if anyone who has UDF for those functions please send me here or at: homayoonsohrabi@yahoo.com thanks for any help 

March 8, 2021, 05:35 
UDF for slip flow in microchannels

#15 
New Member
Join Date: Sep 2020
Posts: 4
Rep Power: 5 
i want to add alternate slip and no slip boundary condition for studying fluid flow 2D microchannels . I wish to get slip length .what UDF should i use.


October 15, 2021, 04:35 

#16 
New Member
Xin Zhang
Join Date: Oct 2021
Posts: 2
Rep Power: 0 
Hi, Dave. I read your UDF and I am working on a slip wall simulation too. The problem confuse me is that when we define the slip wall boundary, a Specified Shear sholud be defined in fluent. How can you write a UDF of the Shear Stress? Does your UDF work well now? Thanks a lot.


Thread Tools  Search this Thread 
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
mixed inflow/outflow downstream boundary condition question  peob  OpenFOAM Running, Solving & CFD  3  February 3, 2017 11:54 
Resolved: Changing boundary condition with UDF according to pressure outlet boundary  alpemre  Fluent UDF and Scheme Programming  12  February 24, 2014 11:18 
An error has occurred in cfx5solve:  volo87  CFX  5  June 14, 2013 18:44 
Boundary Condition Types Using Scheme and UDF  Nasir  FLUENT  0  September 15, 2008 22:54 
UDF : boundary condition ID  Flav  FLUENT  4  June 28, 2001 10:52 