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

Help !!! CFX4.2 users

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

Reply
 
LinkBack Thread Tools Display Modes
Old   November 11, 1999, 00:33
Default Help !!! CFX4.2 users
  #1
Athar Zaidi
Guest
 
Posts: n/a
I am having lots of trouble modeling non-Newtonian turbulent flow with Low-Reynolds number k-omega model ( Wilcox 1993) through stenosed arteries segments , either the values of omega and K decreases to unsual values , something of the order of 10e-40 or the solution blows up. I am using CFX 4.2 ( Aea Technology) CFD solver which is a finite volume based solver. I specify my strain rate based viscosity in USRVIS subroutine and set VISN(INODE,IPHASE) =Vlaminar+Vturbulent. It seems to me that nobody has done a simulation of non-Newtonian turbulent blood flow using low-Reynolds number model till now. However I get some good results with high Reynolds number RNG K-epsilon model, but my flow operates at Reynolds number below 10000. I was wondering if Any one has any clue that may be K-Omega model has a deficiency in this respect, I mean modeling strain rate based viscosity. I couldn`t find such deficiency in literature so far.Please reply soon.
  Reply With Quote

Old   November 11, 1999, 04:03
Default Re: Help !!! CFX4.2 users
  #2
John Chien
Guest
 
Posts: n/a
(1). I don't use the code, so, I can't answer your code related questions. Since you apparently know the vendor of the code, I would suggest that you send them e-mail about your problem. (2). About the questions related to the Wilcox turbulence model, you can follow the same e-mail approach. I think, his address can be found in the Resources section. Actually, he has written a popular book "Turbulence Modeling for CFD", may be you can also find some answers in the book. (3). Since you are interested in getting the solution for Reynolds number lower than 10000, why not just write your own code and then most of your problems would be gone. (4). My suggestion is : if you can't beat them, join them; if you can't get commercial answer, solve them. I think, CFD is a fun field, playing a commercial CFD code like a computer game don't seem to be fun at all.
  Reply With Quote

Old   November 11, 1999, 05:02
Default Re: Help !!! CFX4.2 users
  #3
Gert-Jan van der Gulik
Guest
 
Posts: n/a
Have you used bounded differencing schemes, like 'quick' or 'ccct'? These prevent turbulence parameters to become negative, which might be a problem in your case.

Good luck, Gert-Jan van der Gulik
  Reply With Quote

Old   November 11, 1999, 10:40
Default Re: Help !!! CFX4.2 users
  #4
Joakim Majander
Guest
 
Posts: n/a
I have run into a similar problem. I was using standard k-e model with CFX4.2. In one cell epsilon reached a very small value and the effective viscosity became very large. The simulation blew up in a few iteration after this. The solution was to limit the viscosity. If your k is very small, there is no turbulent viscosity! You may even need to give some balancing source terms to k and w in order to keep them at reasonable values. In my case the limitters were needed only in the beginning of the simulation.

Non-Newtonian fluids and turbulence models are not a good combination. What shear rate (shear rate of mean flow vs. shear rate in the eddies) should you use in the viscosity formula? What viscosity should you use in the turbulence model and wall functions?....
  Reply With Quote

Old   November 12, 1999, 12:40
Default Re: Help !!! CFX4.2 users
  #5
Michael R. Rasmussen
Guest
 
Posts: n/a
Joakim Majander has a good point: How do we in reality separate viscosity from turbulence and solid/fluid interactions. In situations where we have a turbulent non-newtonian fluid - how do we measure stresses correctly and are they equal to the Reynolds stresses ? That is why CFX 4.2 do not allow non-newtonian flows to be turbulent (and why you have work around this restriction by writing the routine yourself). So even if you wrote the whole code from the start - as John suggest - you will still have to answer the questions: What is rheology and how does it interact with turbulence.

I surpose that it is blood you are simulating. Your instrument for measuring the non-newtonian properties of blood should in principle not include the turbulent effect (most intrepetadions of viscometer results assumes laminar conditions). However, it is problematic how the blood plates influence the fluid. It is found that - depending on the rheological properties - the Reynolds number is lower for non-newtonian fluid than for newonian fluids in same geometries and mass flow conditions. This means that flows which are transitional for water can be laminar for a non-newtonian fluid. We also know that particles in water can dampen turbulence (I also heard that they can enhance turbulence in some cases) which all in all makes this kind of problems a mess - or an interesting field of reseach depending on your attitude.

The solution to this problems i'm presently leaning towards is a two-phase model : one for the fluid (turbulent) and one for the "solid" phase which is laminar and non-newtonian. The two phases exchange momentum through a interphase momentum transfer term. The combined phases have to behave like a non-newtonian fluid under laminar conditions which requieres some creative adjustment of the interphase drag coefficient. However, it is problematic the make a good physical justification for this approach as it is difficult (impossible ?)to get good experimental validation. How large should the "solid" phase be ? and how much water is associated to the solids in the water ? and so on. So I guess - my solution is not better than yours.

I would suggest that you supplement your study with experimental validation. Set up some artificial stenosed arteries segments and measure pressuredrop and velocities with LDA.

Regards

Michael
  Reply With Quote

Old   November 16, 1999, 16:59
Default Re: Help !!! CFX4.2 users
  #6
jy
Guest
 
Posts: n/a
Everybody is doing blood flow simulation this days!!

I have done some with the Casson model and the power law model with CFX5.

Everything went OK, providing a mesh adapted to the wall function.

What I would say is: ensure that your velocity profile is well calculated (validated) with the Newtonian corresponding flow (assymptote of the Casson model). Then re-run the simulation with you model.

I don't really know how to input NN model CFX4.2 (CFX4.3 now actually) but with CFX5 it is straigh forward.

cheers

jy
  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
OF installation for multiple users mirko OpenFOAM Installation 0 June 24, 2010 10:52
New dedicated forum for EFD and FloWorks users Forum Administrator Main CFD Forum 6 April 15, 2008 11:56
500 registered CFD-Wiki users Jonas Larsson CFD-Wiki 4 December 9, 2005 12:02
Fluent 5.5. What the differences with fluent 5.3?? confused FLUENT 2 July 29, 2001 21:58
2000 North American STAR-CD Users Conference Andrew Robertson CD-adapco 0 March 31, 2000 18:18


All times are GMT -4. The time now is 04:35.