[liliana]

Hi all,

does anyone here works with NonNewtonian fluids?

I implemented a UDF for calculate the viscosity for a Bingham fluid in a 2D pipe. As BC at inet, I set a pressure 58.86 Pa and at outlet P = 0.

The geometry has 0.002m radius and 0.006m length. The flow is laminar, steady state.

However, when I compare the results of Fluent with analytical solution, it does not match (see picture, there 3 graphs for different values of yield stress). I am not sure if the problem is the UDF. Does anyone have any idea of can be wrong or has the same problem?

k = 1 Pa.s
tau0 = 1.0; 3.0; 5.0 Pa (three simulations with three differente values)

The theoretical equations:

v = (dP/dL) * (R² - r²)/(4*k) - tau0*(R-r)/k (for non-plug region)

v = (dP/dL) * (R²/4*k) * (1 - Rp/R)^2 (for plug region)
with Rp = 2*L*tau0/dP

The picture: https://drive.google.com/open?id=1tn...UYPuTsV6sWnoRE

Here are the UDF:

/* UDF for Bingham fluid (Bingham Papanastasiou model)*/
#include "udf.h"

FILE *fp;


/* ************************************************* */

/* Bingham Fluid */

DEFINE_PROPERTY(Bingham_viscosity, c, t)

{

/* Input Parameters for Bingham Viscosity */

real vis;
real stress;
real ys;
real m;
real k;
real Max, Min;

ys = 5.0; /* Initial Yield Stress */
k = 1.0; /* Fluid Consistency */
m = 100000000;

Max = 100000000000;
Min = 0.00000000001;

stress = C_STRAIN_RATE_MAG(c,t);

/************ Bingham Fluid **********/

vis = k + ys*(1-exp(-m*stress))/stress;
/* vis = k; */

return vis;

}

[blackmask]

Make sure that you have done

solve/set/expert
Keep temporary solver memory from being freed?

and answered "yes".

The picture is inaccessible.

[liliana]

Originally Posted by blackmask

Make sure that you have done

solve/set/expert
Keep temporary solver memory from being freed?

and answered "yes".

The picture is inaccessible.

Hi! What does this code mean? I didnt get it, sorry... I guess the picture is accessible now.

[blackmask]

Simple type "solve/set/expert" in the TUI (text user interface) when you have to access gradient in your UDF. Also, it would be great to post the formulation of viscosity for Bingham flow. I can see what you code does, but I do not know what the code is supposed to do.

[liliana]

Originally Posted by blackmask

Simple type "solve/set/expert" in the TUI (text user interface) when you have to access gradient in your UDF. Also, it would be great to post the formulation of viscosity for Bingham flow. I can see what you code does, but I do not know what the code is supposed to do.

I got it. I will try this. But what this command do exactly?

About the viscosity, I am trying to implement the equation (6) of this paper: https://drive.google.com/file/d/1gQ-...w?usp=drivesdk

[blackmask]

Well in this case you do not have to do that because the viscosity is needed in the momentum equation in which the strain rate is readily available. I think what you have done is right and the discrepancy when plug flow region appears is rather strange. However it might not be easy to figure out why. You might do a full 3D simulation to make sure that this is not an issue with the axis-symmetric implementation in FLUENT.

[liliana]

Originally Posted by blackmask

Well in this case you do not have to do that because the viscosity is needed in the momentum equation in which the strain rate is readily available. I think what you have done is right and the discrepancy when plug flow region appears is rather strange. However it might not be easy to figure out why. You might do a full 3D simulation to make sure that this is not an issue with the axis-symmetric implementation in FLUENT.

I thought about it. But then I made a simulation without axisimetric, but still 2D, as a flow between two paralell plates. And I got the same problem.

[saoYT]

Hello liliana!

I'm currently facing the same problem as you, working with Herschel-Bulkley fluids with ANSYS Fluent.

The Herschel-Bulkley rheological model (for n = 1, we have the Bingham model) has a discontinuity on its function, since we have a yield stress. So, Fluent implements a regularization model to overcome this discontinuity (documented in the user's guide), using a "critical shear rate", which means that for shear rate < critical shear rate, the fluid will behave as a Newtonian Fluid with high viscosity, and for shear rate > critical shear rate the fluid will behave as a Herschel-Bulkley fluid (or Bingham fluid, in your case).

The udf you are showing makes a different regularization for this problem, with the Papanastasiou Model, which depends on the "m" parameter. The literature recomends m = 1000s (LABSI, 2016, "Herschel-Bulkley fluid flow within a pipe by taking into account viscous dissipation"), however i'm not fully convinced about it and i think the "m" parameter needs to be calibrated as well.

I recommend using the fluent's implementation with critical shear rate using low values, in the order of 0.001 s^-1 and 0.01 s^-1, then confront with analytical results as you did.

Any further questions regarding to non-Newtonian fluids, you can PM me.

[liliana]

Originally Posted by saoYT

Hello liliana!

I'm currently facing the same problem as you, working with Herschel-Bulkley fluids with ANSYS Fluent.

The Herschel-Bulkley rheological model (for n = 1, we have the Bingham model) has a discontinuity on its function, since we have a yield stress. So, Fluent implements a regularization model to overcome this discontinuity (documented in the user's guide), using a "critical shear rate", which means that for shear rate < critical shear rate, the fluid will behave as a Newtonian Fluid with high viscosity, and for shear rate > critical shear rate the fluid will behave as a Herschel-Bulkley fluid (or Bingham fluid, in your case).

The udf you are showing makes a different regularization for this problem, with the Papanastasiou Model, which depends on the "m" parameter. The literature recomends m = 1000s (LABSI, 2016, "Herschel-Bulkley fluid flow within a pipe by taking into account viscous dissipation"), however i'm not fully convinced about it and i think the "m" parameter needs to be calibrated as well.

I recommend using the fluent's implementation with critical shear rate using low values, in the order of 0.001 s^-1 and 0.01 s^-1, then confront with analytical results as you did.

Any further questions regarding to non-Newtonian fluids, you can PM me.

Hi! Thanks for the reply! I have tried the model implemented on Fluent already and I got the same result as I got with my UDF...

[saoYT]

Originally Posted by liliana

Hi! Thanks for the reply! I have tried the model implemented on Fluent already and I got the same result as I got with my UDF...

which values did you input at the critical shear rate?

and about the numerical details: which convergence criteria and number of iterations are you using? and where are you getting the velocity data in the domain (usually it's a point/line/plane where the flow is fully developed)?

[liliana]

Originally Posted by saoYT

which values did you input at the critical shear rate?

and about the numerical details: which convergence criteria and number of iterations are you using? and where are you getting the velocity data in the domain (usually it's a point/line/plane where the flow is fully developed)?

I have used 0.1, 0.01, 1e-6, 1e-16... And the results were very very similar..

I am getting the velocity at x=0.045 m, the pipe has x=0.049m. I saw that the flow is fully developed (since I am using a pressure condition at inlet as well....).

I have disable the convergence criteria and I am monitoring the maximum velocity (and the field, and the profile...), when they are stable, I stop the simulation (around residuals 1e-8 or 1e-9).

[saoYT]

Originally Posted by liliana

I have used 0.1, 0.01, 1e-6, 1e-16... And the results were very very similar..

I am getting the velocity at x=0.045 m, the pipe has x=0.049m. I saw that the flow is fully developed (since I am using a pressure condition at inlet as well....).

I have disable the convergence criteria and I am monitoring the maximum velocity (and the field, and the profile...), when they are stable, I stop the simulation (around residuals 1e-8 or 1e-9).

ok, it seems fine.

give a look at this article, the author did a very similar case with fluent and it's well explained.

https://www.sciencedirect.com/scienc...92687514003677

[liliana]

Originally Posted by saoYT

ok, it seems fine.

give a look at this article, the author did a very similar case with fluent and it's well explained.

https://www.sciencedirect.com/scienc...92687514003677

Thanks, I'll take a look!