CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   OpenFOAM (http://www.cfd-online.com/Forums/openfoam/)
-   -   viscoelasticFluidFoam (http://www.cfd-online.com/Forums/openfoam/67668-viscoelasticfluidfoam.html)

ternik August 22, 2009 12:44

viscoelasticFluidFoam
 
1 Attachment(s)
Hi Foamers,

Although that certain amount of test cases have been performed by Jovani in his Master Thesis, I am currently testing viscoelasticFluidFoam in 2-dimensional geometry. For this reason I have simulated so called "start-up flow" of Newtonian and UCM (Upper Convected Maxwell) fluid; it is a transient flow resulting from a sudden application of a spatially constant pressure gradient to a fluid initially at rest as well as a good example of time-dependent flow problem amenable to exact mathematical analysis. More can be found in this article:

A.S.R. Duarte, A.I.P. Miranda, P.J. Oliveira. Numerical and analytical modeling of unsteady viscoelatics flows: The start-up and pulsating test case problem. J. Non-Newtonian Fluid Mech. 154 (2008) 153-169

In this analysis I have used:
  • icoFoam for Newtonian fluid
  • viscoelasticFluidFoam for UCM fluid with two values of relaxation time; 1.0e-08s (Newtonian fluid with almost zero relaxation time) and 1.25s
Comparison of particular results (obtained with icoFoam and viscoleasticFluidFoam) with theoretical expressions (from above mentioned article) yields the following:
  • icoFoam (Newtonian fluid) produces results that are in good (if not excellent) agreement with "theory"
  • viscoelasticFluidFoam (UCM fluid with rel. time 1.0e-08s and 1.25s) produces results that are not near theoretical values.
Here are short details of numerical set up:
  • two-dimensional and time-dependent channel flow (L=2, H=1)
  • constant pressure drop according to the value of Re number (=Ro*V*H/Eta) 10 and length of a channel
  • Inlet B.C. ==> fixeValue for pressure, pressureInletVelocity for velocity, zeroGradient for tau and taufirst
  • Outlet B.C. ==> fixeValue for pressure, zeroGradient for velocity, tau and taufirst
As a "good citizen" I have attached all examples (with "basic files") together with results!

Can anyone (maybee Jovani or Hrvoje) take a look at this and make comments? I hope that I am doing something wrong rather than...

Enjoy the weekend,
Primoz.

anon_c August 24, 2009 05:29

hi hello

i am also very very interessted in non newtonian fluids, the work of Jovani is really great there are more than one or two modells

but to you thank you for this data of cases i will study them very intensiv and wirte back

good job :)

ternik August 24, 2009 05:53

Quote:

Originally Posted by Tajoooko (Post 227253)
hi hello

i am also very very interessted in non newtonian fluids, the work of Jovani is really great there are more than one or two modells

but to you thank you for this data of cases i will study them very intensiv and wirte back

good job :)

Hi Tajoooko,

thanks for showing interest on this subject. Yes, thanks to Jovani (and I think also to Hrvoje) there are many viscoelastic models to be used in... "Imagination is the limit"!

I always (especially, when I am dealing with something new; i.e. OpenFoam, solvers) try to test and validate numerical code, numerical procedure, models... Therefore I think such a test case involving viscoelasticFluidFoam is of great importance not only for me but for everybody out there who is (or will) dealing with viscoelastic fluids!

Looking forward for your reply!

Enjoy,
Primoz.

RayExt September 2, 2009 19:52

These validation / verification activities are excellent.

Unfortunately, the way many of the validation activities take place, it does not tell if it represents "Real Life" scenarios.

My team is currently working with the Viscoelastic solver. We are trying to see how well it predicts real life extrusion problems. We are actually working backwards from the product back to the die configuration to understand just how the model variables interact with the product. (This is a highly simplified summary.)

To date, we have not encountered any software that truly assists us in the design of complex die configurations. Software such as PolyFLOW, CompuPlast, etc.., have only been mildly effective. Much of it has to do with the proprietary and "closed" nature of the software. We are unable to truly correlate the results to the product. In sum, when the die gets on the floor, there is still lots of die modifications that take place.

Unfortunately, none of us have 1/2 the intelligence of those of you posting on this website. So what I can offer to the community is "shop floor" results of the experiments. I just hope that the information I provide is something that is useful for the development of the solvers.

If I am not mistaken, that is the whole point of OpenFOAM. Cost savings, cost avoidance, and continuous improvement.

Ray

jovani October 28, 2009 08:50

Hello Primoz,

Sorry for the delay, I most often see the "Viscoelastic Fluid Flows using OpenFOAM The solver viscoelasticFluidFoam" because the advertise by email to replies. But let's to your problem:
Your case is well defined and for obtain the Newtonian behavior to UCM lambda zero (1e-8 s) case the only changes needed is in relaxationFactors and time step. relaxationFactors make the convergence easy but for unsteady cases this changes the transient solution response, then:

relaxationFactors
{
// U 0.5;
// taufirst 0.3;
}

For have convergence without relaxation you need make the time step (maxDeltaT) smaller, I think 1e-4 is enough.

The UCM is numerically complicated and psychically not good when compared with PTT, Giesekus, ... . When you simulate UCM lambda not zero problems can occurs, and is better to start with smaller elasticity cases before go on in a new stage.


Jovani

ternik October 28, 2009 10:48

Quote:

Originally Posted by jovani (Post 234332)
Hello Primoz,

Sorry for the delay, I most often see the "Viscoelastic Fluid Flows using OpenFOAM The solver viscoelasticFluidFoam" because the advertise by email to replies. But let's to your problem:
Your case is well defined and for obtain the Newtonian behavior to UCM lambda zero (1e-8 s) case the only changes needed is in relaxationFactors and time step. relaxationFactors make the convergence easy but for unsteady cases this changes the transient solution response, then:

relaxationFactors
{
// U 0.5;
// taufirst 0.3;
}

For have convergence without relaxation you need make the time step (maxDeltaT) smaller, I think 1e-4 is enough.

The UCM is numerically complicated and psychically not good when compared with PTT, Giesekus, ... . When you simulate UCM lambda not zero problems can occurs, and is better to start with smaller elasticity cases before go on in a new stage.


Jovani


Hey Jovani,

what a nice surprise :)! Thanks for your comments - I will consider them and I hope for the best. Will keep you (and other OF users) informed...

Wish U all the best,
Primoz.

ternik November 1, 2009 05:31

Quote:

Originally Posted by RayExt (Post 228332)
These validation / verification activities are excellent.

Unfortunately, the way many of the validation activities take place, it does not tell if it represents "Real Life" scenarios.

My team is currently working with the Viscoelastic solver. We are trying to see how well it predicts real life extrusion problems. We are actually working backwards from the product back to the die configuration to understand just how the model variables interact with the product. (This is a highly simplified summary.)

To date, we have not encountered any software that truly assists us in the design of complex die configurations. Software such as PolyFLOW, CompuPlast, etc.., have only been mildly effective. Much of it has to do with the proprietary and "closed" nature of the software. We are unable to truly correlate the results to the product. In sum, when the die gets on the floor, there is still lots of die modifications that take place.

Unfortunately, none of us have 1/2 the intelligence of those of you posting on this website. So what I can offer to the community is "shop floor" results of the experiments. I just hope that the information I provide is something that is useful for the development of the solvers.

If I am not mistaken, that is the whole point of OpenFOAM. Cost savings, cost avoidance, and continuous improvement.

Ray

The purpose of such a validation tests are only (mainly) to test and validate numerical codes - and comparison with theoretical expressions (if they exist at all) is the best opportunity to do that! Of course such a validation (or test) cases are most likely "far away" from real-life scenarios, but on the other hand they give us enough confidence in a numerical tool that is used for making such predictions...

It is my opinion that only after particular numerical code is well tested and validated (if possible) one should proceed with improving existing or developing new models (viscoelastic, turbulence, heat transfer...) to get to the nature as close as possible. And here I see the experiments as the indispensable tool - comparing numerical results for improved models with experimental one will tell us how good this new (better etc.) model is! Last but not least, if test and validation cases are performed carefully one will not have to question if the numerical code is performing well...

So, such a test and validation cases will not resolve "real life scenarios", but they will offer enough confidence in OpenFoam and I see this as useful and important contribution.

Regards,
Primoz.

ternik November 2, 2009 16:22

3 Attachment(s)
Quote:

Originally Posted by jovani (Post 234332)
Hello Primoz,

Sorry for the delay, I most often see the "Viscoelastic Fluid Flows using OpenFOAM The solver viscoelasticFluidFoam" because the advertise by email to replies. But let's to your problem:
Your case is well defined and for obtain the Newtonian behavior to UCM lambda zero (1e-8 s) case the only changes needed is in relaxationFactors and time step. relaxationFactors make the convergence easy but for unsteady cases this changes the transient solution response, then:

relaxationFactors
{
// U 0.5;
// taufirst 0.3;
}

For have convergence without relaxation you need make the time step (maxDeltaT) smaller, I think 1e-4 is enough.

The UCM is numerically complicated and psychically not good when compared with PTT, Giesekus, ... . When you simulate UCM lambda not zero problems can occurs, and is better to start with smaller elasticity cases before go on in a new stage.


Jovani


Hi Jovani,

good and bad news :)! I have followed your recommendations and here are the results (observations) for start-up flow in channel:
  • results for Newtonian fluid (UCM, Lambda= 1.0e-08) are now in excellent agreement with theoretical expressions
  • results for UCM (Lambda=0.05) are also in excellent agreement with theory
  • results for UCM fluid with higher values of relaxation does not follow theoretical predictions
Looks like that something happens with the solution for higher values of relaxation times! I feel that something strange is going on in the pressure-velocity coupling! Why?

I have done the following numerical test - developing flow in a (2-dimensional) channel, uniform velocity and zero pressure gradient at the inlet, zero velocity gradient and zero pressure at outlet, etc. For relaxation time 0.1 (and higher) the following happened with pressure field results:
  • negative pressure values!
  • pressure increases from inlet to outlet (e.g. from -20000 to -10 - O.K., these values are for illustration only)!
Any comments...

Thanks,
Primoz.

jovani November 5, 2009 10:31

2 Attachment(s)
Quote:

Originally Posted by ternik (Post 234869)
Hi Jovani,

good and bad news :)! I have followed your recommendations and here are the results (observations) for start-up flow in channel:
  • results for Newtonian fluid (UCM, Lambda= 1.0e-08) are now in excellent agreement with theoretical expressions
  • results for UCM (Lambda=0.05) are also in excellent agreement with theory
  • results for UCM fluid with higher values of relaxation does not follow theoretical predictions
Looks like that something happens with the solution for higher values of relaxation times! I feel that something strange is going on in the pressure-velocity coupling! Why?

I have done the following numerical test - developing flow in a (2-dimensional) channel, uniform velocity and zero pressure gradient at the inlet, zero velocity gradient and zero pressure at outlet, etc. For relaxation time 0.1 (and higher) the following happened with pressure field results:
  • negative pressure values!
  • pressure increases from inlet to outlet (e.g. from -20000 to -10 - O.K., these values are for illustration only)!
Any comments...

Thanks,
Primoz.

Hello Primoz,

As UCM is a problematic model in the numerical point of view, this is not a surprise find cases witch the solution diverges. For 2D simulations exists a limit of De for UCM model and this limit depend of some subjects as is pointed in the article you mentioned and others too. Going up of this limit introduces instabilities problems not only on pressure-velocity coupling, but takes the problem as a whole to break up, and producing bad (wrong) results.
Using your geometry and your mesh the max. value of lambda without numeric problems is 0.5 s with adjusting some simulations parameters. Changing your mesh to get delta x / delta y bigger and making the dimensions in x bigger you can get a solution to lambda 1.25 s (and it is not a very good solution, the is a little oscillation). See the files.

Attachment 1425

Attachment 1426

We are working to get a method more stable that DEVSS and I believe this will be used to get better transient results too.

Best,

Jovani

ternik November 5, 2009 11:16

Quote:

Originally Posted by jovani (Post 235213)
Hello Primoz,

As UCM is a problematic model in the numerical point of view, this is not a surprise find cases witch the solution diverges. For 2D simulations exists a limit of De for UCM model and this limit depend of some subjects as is pointed in the article you mentioned and others too. Going up of this limit introduces instabilities problems not only on pressure-velocity coupling, but takes the problem as a whole to break up, and producing bad (wrong) results.
Using your geometry and your mesh the max. value of lambda without numeric problems is 0.5 s with adjusting some simulations parameters. Changing your mesh to get delta x / delta y bigger and making the dimensions in x bigger you can get a solution to lambda 1.25 s (and it is not a very good solution, the is a little oscillation). See the files.

Attachment 1425

Attachment 1426

We are working to get a method more stable that DEVSS and I believe this will be used to get better transient results too.

Best,

Jovani

Jovani,

many thanks for your extensive explanation!

Cheers,
Primoz.

amin144 February 5, 2012 07:00

Dear Primoz
 
Hi Dear Primoz
My thesis is just studying this problem and ossilations.
Do you think that Jovani answer is persuasive?
After all, could you improved the results and convince yourself that OF is work correctly in this case?

jortega May 23, 2013 11:32

Quote:

Originally Posted by ternik (Post 227180)
Hi Foamers,

Although that certain amount of test cases have been performed by Jovani in his Master Thesis, I am currently testing viscoelasticFluidFoam in 2-dimensional geometry. For this reason I have simulated so called "start-up flow" of Newtonian and UCM (Upper Convected Maxwell) fluid; it is a transient flow resulting from a sudden application of a spatially constant pressure gradient to a fluid initially at rest as well as a good example of time-dependent flow problem amenable to exact mathematical analysis. More can be found in this article:

A.S.R. Duarte, A.I.P. Miranda, P.J. Oliveira. Numerical and analytical modeling of unsteady viscoelatics flows: The start-up and pulsating test case problem. J. Non-Newtonian Fluid Mech. 154 (2008) 153-169

In this analysis I have used:
  • icoFoam for Newtonian fluid
  • viscoelasticFluidFoam for UCM fluid with two values of relaxation time; 1.0e-08s (Newtonian fluid with almost zero relaxation time) and 1.25s
Comparison of particular results (obtained with icoFoam and viscoleasticFluidFoam) with theoretical expressions (from above mentioned article) yields the following:
  • icoFoam (Newtonian fluid) produces results that are in good (if not excellent) agreement with "theory"
  • viscoelasticFluidFoam (UCM fluid with rel. time 1.0e-08s and 1.25s) produces results that are not near theoretical values.
Here are short details of numerical set up:
  • two-dimensional and time-dependent channel flow (L=2, H=1)
  • constant pressure drop according to the value of Re number (=Ro*V*H/Eta) 10 and length of a channel
  • Inlet B.C. ==> fixeValue for pressure, pressureInletVelocity for velocity, zeroGradient for tau and taufirst
  • Outlet B.C. ==> fixeValue for pressure, zeroGradient for velocity, tau and taufirst
As a "good citizen" I have attached all examples (with "basic files") together with results!

Can anyone (maybee Jovani or Hrvoje) take a look at this and make comments? I hope that I am doing something wrong rather than...

Enjoy the weekend,
Primoz.

Dear Primoz,

I would like to know if you finally got a good comparison with the "start-up flow" of an Oldroyd-B fluid in a channel. I am trying to carry out the same simulations than you (but some years later) and I have some convergence problems.

Thanks in advance for any information.

Cheers,
Joaquin.

NickolasPl February 3, 2014 15:48

Hello everyone,

I understand the nature of tau BC as it is a symmetric tensor of the total stress (elastic+solvent...correct me if I'm wrong here!).

In my problem (in which I use the single phase viscoelasticFluidFoam)I need to set boundary condtions on a free surface. Trying to model the problem as close as to reality I use on the same boundary the following BCs for p and U:

p=0
U=slip (shear free surface with no cross flow)

In the same manner I need to set the BC for tau. I have searched so far in the tutorials and found out that this BC can have the following types:

type fixedValue;
value uniform (0 0 0 0 0 0);

or

type zeroGradient;

In my case which is 2D some tensor elements of tau are a priori zero (since I put "empty" patches). From the rest elements, and since the boundary behaves as s free surface not all of them must be zero.

My question is: How can I let openFOAM calculate only specific elements of the tensor and let the rest be zero?? I tried so many many times the directionMixed BC but in vain. I would appreciate your support regarding this matter.

Regards,

Nickolas


All times are GMT -4. The time now is 00:52.