# UDF for slip boundary condition

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

 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 (0.0001-0.005) 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 BARKAT likes this.

 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 Low-Pressure 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 low-pressure 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:
 Originally Posted by m zahid 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,
Please read the messages in this thread more carefully. If you would have done that, you would not have asked for a UDF.

 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.cfd-online.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 under-relaxation is required for the calculated tangential wall velocity . BTW: The formula for Maxwell-based Slip Boundary Formulation for Low-Pressure 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 auto-calculated 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 user-defined memories (UDM) need to be allocated first! =============================================== */ // wall slip layer thickness [m] #define DELTA 10.0e-6 // under-relaxation 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 face-id 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 = (1-RELAX_CT)*F_UDMI(face,f_thread,0)+RELAX_CT*DELTA*gamma; // calculate tangential velocity (with under-relaxation using previous calculation step) F_UDMI(face,f_thread,0)=ct; //store in user-defined face memory (id=0) for next calculation cx = ct*u/sqrt(u*u+v*v); // component of ct in x-direction 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 = (1-RELAX_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) } NonStopEagle and by1704116 like this.

 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 liquid-solid 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.