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

Turbulent flow of non-Newtonian fluids

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

Reply
 
LinkBack Thread Tools Display Modes
Old   January 23, 2014, 19:11
Default Turbulent flow of non-Newtonian fluids
  #1
New Member
 
Majid
Join Date: Jan 2014
Location: Canada
Posts: 17
Rep Power: 2
sharif88 is on a distinguished road
Hi everyone
I am kind of new to CFX, and I have this case where I have to simulate turbulent flow a power law type fluid.
My simulation works perfectly for water but when it comes to the polymer solution I cannot get good results,
pressure loss increases while it should decrease (drag reduction)
What I did was just defining a new material with the transport property defined as the rheology model I had,
I appreciate if any of you could give me hint to how to tackle this problem,
Thanks in advance
sharif88 is offline   Reply With Quote

Old   January 27, 2014, 18:14
Default
  #2
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 9,716
Rep Power: 77
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
Turbulence modelling on non-Newtonian fluids is a complex subject and an area of research. There are no simple models in this flow regime. If you choose to model this type of flow you should expect difficulties in convergence and very inaccurate simulations.

My only suggestion is you need to go to the literature and find what other people have done in this situation.
ghorrocks is offline   Reply With Quote

Old   January 27, 2014, 18:24
Default
  #3
New Member
 
Majid
Join Date: Jan 2014
Location: Canada
Posts: 17
Rep Power: 2
sharif88 is on a distinguished road
ghorrocks Thanks for your advise, what I have learned so far is that this type of fluids may be well represented as a multi-phase fluid, the interaction between polymer molecules and water however is difficult to simulate as drag reduction phenomena is not well understood itself,
DNS guys use some sort of elastic models to simulate shear thinning fluids, I don't know if CFX is capable of modeling this type of interactions,
If I get any success I'll post that,
Thanks
sharif88 is offline   Reply With Quote

Old   February 11, 2014, 05:14
Default
  #4
Member
 
Naimah
Join Date: Nov 2011
Posts: 53
Rep Power: 5
wanna88 is on a distinguished road
Hi Ghorrocks,

I did read your comments on the forum and I hope you can give some advice on this.

I have run non Newtonian (Carreau Yasuda model (shear thinning effect) using the UDF) using patient specific geometry (human disease vessel) in FLUENT and compared the pressure drop with the Newtonian model (viscosity : 0.00371 Pa.s).
I cannot see difference (very small difference : approximately less than 1%) in the pressure drop between Newtonian and non Newtonian model.

Then, to ensure the UDF model that have been implemented was correct, I used the ideal geometry (3D simple tube). I can see the pressure drop difference between both cases (~ 7%).

When there are changing in the resistance (viscosity), the pressure drops should be changed isn't it?

Why when I implemented this concept in the patient specific geometry, I cannot see this?

Please advice.

Thank you

Regards,
Naima
wanna88 is offline   Reply With Quote

Old   February 11, 2014, 18:23
Default
  #5
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 9,716
Rep Power: 77
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
FAQ: http://www.cfd-online.com/Wiki/Ansys..._inaccurate.3F
ghorrocks is offline   Reply With Quote

Old   February 17, 2014, 23:57
Default
  #6
Member
 
Naimah
Join Date: Nov 2011
Posts: 53
Rep Power: 5
wanna88 is on a distinguished road
Thank you for the suggestions:

I have tested 3 things:
1) Residual
2) Time step (since it is transient simulation)
3) Mesh/ grid

Attached is the geometry and the tested results.
1) Residual: not much changes for the pressure drop can be seen
2) time step: not much changes for the pressure drop can be seen
3) Mesh/ grid : I can see the pressure drop difference however the results show that the Newtonian has higher pressure drop compare to non Newtonian (Carreau Yasuda) model. Should the other way isn't?

Did my analysis is correctly been done?

Please advice.

Thank you

Naima
Attached Images
File Type: jpg geometry.jpg (20.4 KB, 14 views)
File Type: jpg residual and time step analysis.jpg (60.0 KB, 14 views)
File Type: jpg mesh analysis.jpg (57.5 KB, 11 views)
wanna88 is offline   Reply With Quote

Old   February 18, 2014, 07:36
Default
  #7
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 9,716
Rep Power: 77
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
Quote:
Did my analysis is correctly been done?
Ummmm, no. I think you missed the point. Let me explain.

Forget the non-Newtonian stuff for now. Just look at the Newtonian flow. You ran a residuals convergence of 1e-4 and 1e-6 and it changed the results from 1223 to 1376. This is a change of 10% and most people would not be happy with this. I would run 1e-5 and 1e-7. By 1e-7 I would expect the results to be asymptoting to the fully converged result - so you can choose the convergence which gives you an accuracy you are happy to accept from that.

Likewise, for the time step size you have 13.76, 13897 and 26318. These are massive changes between each run and indicates you are nowhere near a suitable time step size. You need to keep making it smaller until it starts to asymptote to a final value. Again, then you can choose the time step size which gives an accuracy you are happy to accept.

Finally, your mesh size check did not cover a wide enough range. 3.5M nodes versus 2.6M nodes is only a small difference in element edge length. You should be comparing something closer to halving or doubling the element edge length - which results in approximately 8 times more/less nodes in the mesh.

Once you have found a suitable convergence tolerance, time step and mesh then if you want to be thorough you should check sensitivity again because your first check was probably on the wrong mesh, time step or convergence tolerance.

And finally, once you have done all that your Newtonian flow model should be accurate. Now you can repeat it all over again with a non-Newtonian rheology model.
ghorrocks is offline   Reply With Quote

Reply

Tags
drag reduction, non-newtonian, turbulent

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
About Some Concepts:Laminar flow, turbulent flow, steady flow and time-dependent flow Jing Main CFD Forum 5 March 2, 2013 15:02
CFX Treatment of Laminar and Turbulent Flows Jade M CFX 6 January 26, 2013 11:11
Beginner level doubts with turbulent flow simulation setup Sagun OpenFOAM 1 October 22, 2012 10:56
modelling laminar and turbulent flow in the same Ol FLUENT 2 November 25, 2005 03:52
turbulent mixing of two fluids ulrich bieder Main CFD Forum 2 October 9, 1999 17:15


All times are GMT -4. The time now is 13:20.