CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   CFX (http://www.cfd-online.com/Forums/cfx/)
-   -   Turbulent flow of non-Newtonian fluids (http://www.cfd-online.com/Forums/cfx/128912-turbulent-flow-non-newtonian-fluids.html)

sharif88 January 23, 2014 19:11

Turbulent flow of non-Newtonian fluids
 
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

ghorrocks January 27, 2014 18:14

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.

sharif88 January 27, 2014 18:24

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

wanna88 February 11, 2014 05:14

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

ghorrocks February 11, 2014 18:23

FAQ: http://www.cfd-online.com/Wiki/Ansys..._inaccurate.3F

wanna88 February 17, 2014 23:57

3 Attachment(s)
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

ghorrocks February 18, 2014 07:36

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.


All times are GMT -4. The time now is 05:29.