viscoelasticFluidFoam

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

August 22, 2009, 12:44
viscoelasticFluidFoam
#1
Member

Primoz Ternik
Join Date: Apr 2009
Location: Maribor, Slovenia
Posts: 65
Rep Power: 8
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.
Attached Files
 ChannelStartUpFlow.tar.gz (34.2 KB, 105 views)

 August 24, 2009, 05:29 #2 Member   Join Date: Jul 2009 Posts: 63 Rep Power: 7 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

August 24, 2009, 05:53
#3
Member

Primoz Ternik
Join Date: Apr 2009
Location: Maribor, Slovenia
Posts: 65
Rep Power: 8
Quote:
 Originally Posted by Tajoooko 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!

Enjoy,
Primoz.

 September 2, 2009, 19:52 #4 New Member   Ray Join Date: Aug 2009 Posts: 2 Rep Power: 0 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

 October 28, 2009, 08:50 #5 Member   Jovani L. Favero Join Date: Mar 2009 Location: Rio de Janeiro, RJ, Brazil Posts: 41 Rep Power: 9 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

October 28, 2009, 10:48
#6
Member

Primoz Ternik
Join Date: Apr 2009
Location: Maribor, Slovenia
Posts: 65
Rep Power: 8
Quote:
 Originally Posted by jovani 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.

November 1, 2009, 05:31
#7
Member

Primoz Ternik
Join Date: Apr 2009
Location: Maribor, Slovenia
Posts: 65
Rep Power: 8
Quote:
 Originally Posted by RayExt 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.

November 2, 2009, 16:22
#8
Member

Primoz Ternik
Join Date: Apr 2009
Location: Maribor, Slovenia
Posts: 65
Rep Power: 8
Quote:
 Originally Posted by jovani 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)!

Thanks,
Primoz.
Attached Files
 ResultsUCM_Lambda=0.pdf (31.3 KB, 71 views) ResultsUCM_Lambda=0_05.pdf (30.3 KB, 75 views) ResultsUCM_Lambda=1_25.pdf (32.0 KB, 72 views)

November 5, 2009, 10:31
#9
Member

Jovani L. Favero
Join Date: Mar 2009
Location: Rio de Janeiro, RJ, Brazil
Posts: 41
Rep Power: 9
Quote:
 Originally Posted by ternik 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.

Ux_lambda_0.5.jpg

Ux_Lambda_1.25.jpg

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

November 5, 2009, 11:16
#10
Member

Primoz Ternik
Join Date: Apr 2009
Location: Maribor, Slovenia
Posts: 65
Rep Power: 8
Quote:
 Originally Posted by jovani 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.

 February 5, 2012, 07:00 Dear Primoz #11 Member   Amin Shariat KHah Join Date: Apr 2011 Location: Shiraz Posts: 86 Rep Power: 6 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?

May 23, 2013, 11:32
#12
New Member

Joaquin
Join Date: Mar 2009
Location: Málaga, Andalusia, Spain
Posts: 6
Rep Power: 8
Quote:
 Originally Posted by ternik 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.

 February 3, 2014, 15:48 #13 Member   Nickolas P Join Date: Oct 2010 Location: Greece Posts: 30 Rep Power: 6 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

 Tags viscoelasticfluidfoam

 Thread Tools Display Modes Linear Mode

 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 OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

All times are GMT -4. The time now is 07:55.