CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   FLUENT (http://www.cfd-online.com/Forums/fluent/)
-   -   Non-Newtonian Power Law for Viscosity (http://www.cfd-online.com/Forums/fluent/49202-non-newtonian-power-law-viscosity.html)

 John September 6, 2008 14:15

Non-Newtonian Power Law for Viscosity

I am trying to set viscosity to non-newtonian power law for non-newtonian liquid. In the materials panel, the drop down list does not show non-newtonian power law (it shows constant, piecewise linear, piecewise polynomial, polynomial, power law, sutherland, kinetic theory and user defined).

32.3.15 of the user manual states that I should be able to select non-Newtonian power law and then set consistency index, power law index, reference temp, and min & max viscosity limits.

Please advise how I can access the non-newtonian power law function?

 jay September 7, 2008 06:19

Re: Non-Newtonian Power Law for Viscosity

Hi John,

I think you have selected viscous model as turbulent..please change to laminar.

Non newtonian models are available with only laminar viscous models.

 PraveenKumar R September 25, 2008 01:36

Re: Non-Newtonian Power Law for Viscosity

There is no model that can be used for viscosity as we need non-Newtonian power law. To enable the model, issue the text user interface command as:

define/models/viscous/turbulence-expert/turb-non-newtonian> Enable turbulence for non-Newtonian fluids? [no] yes

 Kirill July 15, 2014 05:46

I began to learn the Ansys Fluent and the first task for me - the determining the pressure drop in pipe with non-newtonian fluid.
The Flow mode - turbulent.
I found your post about opportunity to switch turbulence for non-newtonian fluid!

"To enable the model, issue the text user interface command as:

define/models/viscous/turbulence-expert/turb-non-newtonian> Enable turbulence for non-Newtonian fluids? [no] yes"

Can you tell me how to go to the text user interface command mode?

Many thanks!

 ghost82 July 15, 2014 09:49

1 Attachment(s)
Quote:
 Originally Posted by Kirill (Post 501533) I began to learn the Ansys Fluent and the first task for me - the determining the pressure drop in pipe with non-newtonian fluid. The Flow mode - turbulent. I found your post about opportunity to switch turbulence for non-newtonian fluid! "To enable the model, issue the text user interface command as: define/models/viscous/turbulence-expert/turb-non-newtonian> Enable turbulence for non-Newtonian fluids? [no] yes" Can you tell me how to go to the text user interface command mode? Many thanks!
See attached image.
Enter commands in the command window; you have to type define and press enter, then type models and press enter, and so on.

Daniele

 Kirill July 16, 2014 03:49

1 Attachment(s)
Many Thanks for help!

Now I will try to use this option to calculate the flow in the pipe.

Thanks!

 skmaperu November 26, 2014 09:44

I have done the above described thing.
But i couldnot found power law model in models

my intention is to calculate the velocity differences for dilatant and pseudoelastic fluid.

 Simona September 6, 2015 10:34

Hello guys!!! i also have some problems with the non newtonian power law.
First of all i have to specify that I m a beginner in fluent.
I have a Pipe with non Newtonian fluid inside i do not have the lenght of my geometry but my fluid is fully developed (that means that the pipe should be pretty long to have this condition right?)
Well i draw my geometry and than i start to use fluent whe i define material and i put "water-liquid" than i select "viscosity-> Non newtonian power law" and then i should have minimun and maximum viscosity, but i don't, and i really don't know which kind of values i have to put and in which way i can ceck if they will be correct or not?Can you help me please? Thanks.:o

 ghost82 September 11, 2015 08:02

1 Attachment(s)
Hi,
when you chose the power law viscosity for a non newtonian fluid you have to enter the following inputs:

consistency index (k): it is a measure of the average viscosity of the fluid
power law index (n): it represents a measure of the deviation of the fluid from Newtonian
lower limit viscosity eta(min): if the calculated viscosity is lower then eta(min), viscosity will be eta(min)
upper limit viscosity eta(max): if the calculated viscosity is greater then eta(max), viscosity will be eta(max)

If it is temperature dependant, also:
reference temperature (T0)

Power law viscosity is defined as:
eta(min)<eta=k*gamma(dot)^(n-1)*exp(T0/T)<eta(max)

gamma(dot) is the shear rate.

What you call minimum and maximum viscosity are eta(min) and eta(max).

The panel for power law for non temperature dependant viscosity should be as the attached image.

 Simona September 11, 2015 17:22

Hi,
Many thanks for the answer :)
I agree with the minimun but the problem is with the maximum i mean i don' t know where i have to stop:What i mean, i can try with 1000 e my max will be lower or i can try with 100 and the max will be exactly 100 and never happen that the calculated viscosity is greater then the max.
I think that is a convergence problem...but i really don't have any clue how to get it!
I hope that you can help me.

 ghost82 September 12, 2015 03:20

Viscosity is an input parameter, so you must know its equation: lower and upper limits, as you may know, defines the newtonian behaviour of the non-newtonian fluid in that ranges (eta<eta(min), eta>eta(max)).
If you don't have lower-upper limits just input 0 for the lower limit and a high value for the upper limit, greater than the maximum viscosity you expect.
If you don't know what will be the maximum expected viscosity just input a very high value, 1e10 for example.

 Simona September 12, 2015 05:19

I m sorry but i still have some doubts. :( :)
Maybe i was unclear so i will explain you better :
I have to investigate the velocity and pressure and Temperature profile of my NON Newtonian fluid in a tube with some elements inside(they have the own temperature that is different to the initial temperature and close to them the viscosity will decrease).
Well. I know the D of my pipe and the position of each elements and i know that The length is infinite(but obviously i have to define by myself) and i even know that before of my elements i need to have fully developed flow.
I know Re(for non Newtonian fluid of course) so i can calculate the initial velocity.
I draw my geometry in gambit (i decide to fix 1m of lenght ) then when i open fluent and i want define the material i have all parameter except the range of viscosity:
min viscosity:i agree with your explanation

max viscosity : i have to find the right values, because i think that i can 't use one general values i mean my profile will change (and i saw it) every time that i modified the range,that's why i was asking how can i know the maximum? :(
i tried to calculate the velocity profile with a normal tube(without elements) and maybe find the one that could be better ..but the problem is that better compare to what?
and than if in the simple one whatever values of viscosity i choose fluent work, in the other case with really big range fluent show me an error Of divergence.

maybe now that you have all the details for you will be more clear.:)

thanks again:)

 ghost82 September 12, 2015 05:37

1 Attachment(s)
Yes I understand.
The fact is that the eta(max), as the eta(min), is not "to be found", but it must be measured by experimental tests: you must know if, when and where your non newtonian fluid behaves as a newtonian fluid.
Of course when you change the limits viscosity can change (see attached picture).
But you can't input "random" values for these limits, the limits must to be known by experimental.

 Simona September 12, 2015 05:58

ok i got your point , but the problem is that i don't have the opportunity to get the values with experimental test :( because mine is a kind of little project for my career ...so i just need to know how can i choose properly the max... :)

 ghost82 September 12, 2015 06:02

This is a problem :)
You can't run a simulation if you don't know your inputs.
If you can't perform tests with a viscosimeter, I suggest to search in scientific literature to find the shear rate/viscosity curve of your fluid, or find a curve of another fluid which can be approximated to yours.
What is the fluid you are simulating?

 Simona September 12, 2015 06:08

I don't have a real fluid :)..i mean i know that the density of my fluid is the same of the water..and that's it...so even if i want to search something in literature i can t :( ....

 ghost82 September 12, 2015 06:18

mmmmmm.....let's start over....
You have a pipe and a non newtonian fluid flowing in that pipe.
You want that this fluid has a power law viscosity, and you want also that the density of this fluid is 1000 kg/m3.
But, if you are not defining a fluid (you are saying that you haven't a real fluid?) what is the goal of this simulation?
It's ok that you want to simulate a not real fluid, it's quite common: but if it isn't a real fluid you must fix its properties.
If you don't know what is the fluid/properties how can you get velocity/pressure and temperature profiles?these will change with properties!!!

Again, if you want to simulate a generic non newtonian fluid with density of water and power law viscosity, search in scientific literature for a curve approximating the fluid you are searching.

 All times are GMT -4. The time now is 03:06.