VOF-Simulation of Fiber Impregnation - Odd Results

162 Views
Last Post 03 July 2018
Topic Is Solved

eufrat posted this 06 June 2018

Hi guys,

I am working on a simulation of the impregnation of carbon fibers with resin.

For this, I made a multi-phase VOF model with Fluent. At the current state, the model is pretty simple. The carbon fibers are represented by four rigid circles and their motion into the resin is defined by a profile. The two phases which are involved are air and resin. The air is depicted blue, the resin red. Initially, the model consists of four fibers represented by the rigid walls and the surrounding air, the lower part of the geometry is filled with resin. The geometry is really small, the fibers have a diameter of 7 micrometers.

I activated gravity in this model. As viscosity model, I used k epsilon realizable with scalable wall functions.

The behavour of the solution riddles me quite a bit, so I would really appreciate if you could take a look on my solution mpeg which I uploaded on vimeo:

The geometry is completely closed, no pressure outlet or anything. The mpeg depicts the models behaviour for a simulated time span of a whole two hours. Note that I used variable time stepping in this simulation, so since every time step one fram was created, the animation does not depict real time. For example the motion of the fibers into the resin happens in a very short time of only 16 microseconds. The time step was really small at the beginning and began to rise up when the velocities in the model decreased. It grew up to a size of 1 second near the end of the solution.

As one can see, the gravity kind of works strangely in my model. First, there is some kind of whirl building up, which is kind of understandable. But at some point, the resin should move downwards again and the air bubbles in the resin should rise up. This does happen somewhat, but really slowly. I would have expected that to be happened after a fairly long physical time of 7200 seconds.

This is my first simulation with Fluent and my overall knowledge of this software is still pretty basic. If anyone has some thoughts to share on my solution, please be welcomed to do so.

Thanks in advance!

eufrat

#Permalink
0
0
0

15 Comments

Order By: Standard | Newest | Votes

Moderator

raul.raghav posted this 06 June 2018 - Last edited 06 June 2018

A few quick questions:

1. Are you using implicit VOF? VOF is recommended when you have a large interface between the two fluids. So there are good for stratified flows and for tracking large bubble. In this case, the way you've set the simulation, I feel mixture model or the Eulerian model would make a lot more sense. Ansys Fluent theory manual mentions:

For bubbly, droplet, and particle-laden flows in which the phases mix and/or dispersed-phase volume fractions exceed 10%, use either the mixture model or the Eulerian model.

For slug flows, use the VOF model.

For stratified/free-surface flows, use the VOF model.

As discussed in this section, the VOF model is appropriate for stratified or free-surface flows, and the mixture and Eulerian models are appropriate for flows in which the phases mix or separate and/or dispersed-phase volume fractions exceed 10%. (Flows in which the dispersed-phase volume fractions are less than or equal to 10% can be modeled using the discrete phase model.

2. You've set this up as a 2D planar model I'm assuming. Would you be able to post a picture of your mesh?

3. What is the Reynolds number you're looking at? Based on the fiber diameter of 7 micrometers, I doubt if you'll need a turbulent model for this case. And always remember that k-e model does not do well in laminar cases.

Rahul

#Permalink
0
0
0

eufrat posted this 07 June 2018 - Last edited 07 June 2018

Hi Rahul,

1. I am using explicit VOF. I never questioned my choice of the multiphase model... I will try Eulerian and Mixture model, thanks for the heads up

2. Yes, it is 2D planar. I use triangular elements because the dynamic mesh works best with these.

3. I will come back to this question, I need to elaborate on this one a bit. I established a turbulence model because the velocity of the fibers diving in is quite big with 1 m/s, so I thought that turbulence model is possibly needed.

Greetings,

eufrat

#Permalink
0
0
0

eufrat posted this 10 June 2018

Hi again,

I tried the simulation without turbulence model and the results get better. Seems I am better off with laminar and inviscid model for my case.

#Permalink
0
0
0

Moderator

raul.raghav posted this 11 June 2018

Just wondering. How did you come to the conclusion that you could consider it as an inviscid case? Low Reynolds number means that the viscous forces cannot be ignored and assuming inviscid would be a terrible mistake. And I doubt if any of the multiphase problems can be modeled using the inviscid assumption.

An additional information: Its stated in the Theory Guide that the Mixture and Eulerian multiphase models in Fluent cannot be used for inviscid flows. Refer:

Overview and Limitations of the Mixture Model

Overview and Limitations of the Eulerian Model

Rahul

#Permalink
0
0
0

eufrat posted this 12 June 2018

Hi Rahul,

yes, inviscid is clearly inappropiate for my case. But it was nice for me to see that the gravity worked as it should with inviscid modeling. I conclude from that that I have not made a methodic mistake regarding the implementation of gravitational force.

The resin basically behaved similar to water with inviscid modeling. I will upload a video in near future, it takes a little bit of time to compress the files and find a good site to upload it on.

At the moment I am trying to get better results with laminar model. This already looks much more realistic but has still some strange phaenomena in it, a video will follow soon.

Regarding your suggestion to use one of the two other multiphase models: I tried that, but my simulation crashed immediately with mixture and pure Eulerian model. I read into the topic and came to the conclusion that it might surely be wise to try the simulation with another multiphase model, but it can´t be a explanation for these odd physical results I am getting right now. So I put that aside for now and focus on laminar VOF-multiphase.

Currently I am facing hardware wise problems on my working computer so working options are quite limited at the moment. You will hear from me soon.

eufrat

#Permalink
0
0
0

eufrat posted this 12 June 2018 - Last edited 12 June 2018

Sooo, here are two videos:

1. Inviscid with First Order Upwind discretization scheme.

I had to use First Order Upwind for this one because divergence occured. Meanwhile I refined my mesh. The mesh I showed you above had approx. 20.000 elements, the refined mesh has 34.000. Since then I have had no divergence problems so far.

Albeit the fact that inviscid resin has nothing to do with reality, I am pleased that the physical behaviour looks quite plausible.

2. Laminar with Second Order Upwind

The quality of this video is pretty poor. Anyways, the essential physical behaviour is visible. With the refined mesh, the simulation runs really smoothly. Convergence is reached after 2-4 iterations and I have had no aborts so far. But still, the physical behaviour riddles me. This video features the physical behaviour for 120 seconds, and the resin does not go downwards by the gravitational force, which I think should have happened after the quite long time of 120 seconds.

Greetings

eufrat

#Permalink
0
0
0

eufrat posted this 18 June 2018

Hi again,

forget about the last video I posted... While rebuilding the simulation with a finer mesh, I made a mistake in the material assignment of the phases: Both phases are air in the video. The solution is absolute nonsense.

So now I am trying to complete the simulation with the right material assignment. Unfortunately, my simulation diverges pretty quickly (AMG detected divergence in x and y momentum).

I run it with the SIMPLE algorithm. Switching to First Order Upwind did not help, the first try of reducing the relaxation factors didn´t work either (I changed pressure from 0.3 to 0.2, density and body forces from 1 to 0.7 and momentum from 0.7 to 0.5).

I tried PISO algorithm as well, as it is stated in the ANSYS manual that it copes well with transient simulations, but I have not made good experiences with PISO in this simulation so far.

I also tried it with an even finer mesh. I increased the count of elements from 34.000 to 72.000 but it only increases the computational effort and doesn´t bring up any profit regarding the avoidance of divergence.

Maybe someone has another advice for me?

Greetings

eufrat

#Permalink
0
0
0

Admin

Kremella posted this 20 June 2018

Hi,

Have you checked your timestep in your transient simulation? Also, if you have not already tried, I would run the simulation using 'Explicit VOF' settings as opposed to 'implicit' and reduce the time step. The time step should low to maintain a small Courant number. You could find more about this in the Fluent Users Guide (Section 24.3.9).

Hope this helps.

Best Regards,

Karthik

#Permalink
0
0
0

eufrat posted this 20 June 2018

Hi Karthik,

I use variable time stepping with a max. Courant Number of 2 and I already run the simulation in explicit VOF mode.

At the moment I run the simulation with very small relaxation factors of 0.1. Divergence still occures after a few hours.

Thanks for your input!

eufrat

#Permalink
0
0
0

Admin

Kremella posted this 20 June 2018

Hi,

Thank you for your update. I apologize, I didn't read your initial comments on explicit VOF.

Quick thoughts: Did you tried switching off the variable time stepping in your model and use a fixed time step? Also, are you making sure that you have enough iterations per time steps to meet the set residual criteria? You sometimes see divergence because of improper convergence per time steps.

Please let us know your thoughts.

Thank you.

Best Regards,

Karthik

#Permalink
0
0
0

eufrat posted this 20 June 2018 - Last edited 20 June 2018

Hi,

no need for apologizing!

I will try to deactivate the variable time stepping and use a fixed time step. But I am not to optimistic that this will help. The calculation of the time steps every next step by variable time stepping with orientation on the courant number = 2 should result in a pretty conservative time step size, it definetly should be small enough (the time step size is quite small during some periods of the simulation, magnitude e-11). But I will certainly try it.

I have made the experience that some users dont really trust this adaptive time stepping method. So why did I start using it in the first place?

Well, my simulation kind of requires it. A few more notes on my simulation: The lower part is filled with resin initally, the upper part is filled with air. What happens in my simulation is that the rigid circle walls, which represent my fibers, splash into the resin. I have defined the motion of the fibers trough a motion profile. I set the velocity to 1 m/s. The distance which the fibers cover is 16 micrometers, so the motion process happens in 16 microseconds. So during this phase of my simulation, my time step has to be really small, most important for my dynamic mesh not to fold and to make sure that remeshing works well.

When the motion is done, the time step can begin to increase again with regard to the internal velocities, which of course is covered in the Courant Number criteria. Directly after the motion phase, the splashing resin has considerable velocities, so the time step is still in very small regions for a while. But it will increase eventually when the velocities get lower and the system comes into a state of equilibrium again. So basically, with variable time stepping, I want to make sure that the time step is small enough at critical points, but gets considerably higher when the circumstances allow it. This contributes to an acceptable solution time.

Regarding the number of iterations:

I set this to 1000, so this is pretty much. At the beginning of the simulation it takes some more iterations to get convergence, I think he needed about 300 on the first time step. In the following time steps, it converged mostly in the first 30-40 iterations. But there are some fluctuations here and there, and at some point there is a moment when he does not reach convergence at all with 1000 iterations.

I will also try an even higher number, shouldn´t do any damage. Maybe it helps.

Greetings

eufrat

#Permalink
0
0
0

Admin

Kremella posted this 21 June 2018

Hi,

About using variable time steps, its is just my personal choice that I use fixed time-steps and I generally tend to be conservative when selecting it. But more importantly, the simulation has to have sufficient iterations to allow the solution to converge every time step.

Quick questions:

What are the density and viscosity ratios of the two phases?
Are you using PRESTO! for pressure discretization?

Thanks for the updates.

Best Regards,

Karthik

#Permalink
0
0
0

eufrat posted this 21 June 2018

Hi Karthik,

the density ratio is 1100 kg/m³ (resin) to 1,2 kg/m³ (air).

The viscosity ratio is 0.3 Pas (resin) to 1.71 e-5 Pas (air).

Yes, I use PRESTO scheme.

Greetings,

eufrat

#Permalink
0
0
0

eufrat posted this 26 June 2018 - Last edited 26 June 2018

Hi,

a short update: Still struggeling with strange physics in my result.

This simulation depicts the physical behaviour for 10 seconds. It looks like the whole model is kind of in a frozen state after the fibers have dived into the resin. So weird. Now I will reduce the viscosity of the resin by factor 10 and see if this changes anything. Further above I posted a simulation with inviscid multiphase model, this is still the only solution which physically makes sense. My conclusion from this is that my odd results should have something to do with viscosity..

#Permalink
0
0
0

eufrat posted this 03 July 2018

A short update on my simulation again:

I reflected on the approach of the simulation and the strange physics which appear so different from what I expected. There are two possibilities on why the simulation seems to fail for my purpose:

1. There is something wrong with my model

2. My expectations are faulty and the simulation is in fact correct

One thing which I always had to remind me of is that this simulation depicts a tiny, tiny extract from the real situation. The microscopic behaviour of the resin is a whole other story than its macroscopic.

The main problem I have with my simulation results is the fact, that the resin doesn´t seem to bother to flow downwards again after the fibers have diven into the resin. I made a simple test where I put the resin in the upper left corner of the model and deactivated the motion of my fibers to see how the resin reacts to the gravitational force.

This is once again variable time stepping and the simulation depicts the behaviour for a time of 185 seconds.

From this test I concluded, that my model is in fact correct and the resin will eventually flow down again, but it takes quite a long time for this to happen. Since the mass of the resin is really, really small, since its volume is really small as well, the gravitational force needs a lot of time to set the resin, which is holded altogether by its viscosity, into motion.

So as a conclusion, I can state that I expected a physical behaviour which would be provided by a macroscopic simulation model. But since it is a microscopic model, my expectations were simply illusionary.

I have to conclude that this approach is not suited for the purpose it was intended for.

Feel free to comment on what you think of my conclusion and if you think I am right oder not etc. I would really like to read others opinions about this.

I will mark this thread as solved in the meantime.

Greetings

eufrat