Possibilities of Symmetry Boundary Conditions in Fluent

  • Last Post 01 May 2018
eufrat posted this 15 April 2018

Hi guys,

I have a question regarding the possibilities of creating symmetries in ANSYS Fluent.

I desire to simulate the impregnation of fibers with resin. For this purpose, I modelled a geometrically very small domain which contains the cross section of four fibers surrounded by air and the resin beneath them. Please see the image below. As you can see, the fibers are only represented by four rigid circles.


So right now my model is a closed domain, which results in the uprising of the resin level as the four cyclic walls push downwards. Of course, this model is only a tiny cutout of the real situation, in which thousands of fibers get impregnated with resin. In the real impregnation process, the rising of the resin level is nearly negligible, so for my model approach, I don´t want the resin level rising up at all when the fibers push downwards. In other words, the resin which is pushed away by the volume of the circle walls could go anywhere, left, right or downwards (trough the models walls into nirvana or something), but not upwards.

I tried to mark the left and the right wall side as "symmetry" in boundary conditions (the model is perfecty axis-symmetric), but it didn´t have the desired effect. Which didn´t surprise me either, but..

So my question to you guys is: Is this realizable or is it not? Maybe there are other ways to get the model behave as described above?

I am thankful for any input!

Thanks in advance!




Order By: Standard | Newest | Votes
peteroznewman posted this 15 April 2018

Hi eufrat,

I'm slowly learning CFD, and I know some CFD experts will also reply, so take my input as food for thought until they do.

I would set this up without moving any bodies. I would have an inlet of resin just below the fibers, and an outlet for the air above the fibers and use either a velocity or a pressure BC on the inlet to push resin into the fibers. You don't need all the resin in the domain at the start, it can be "created" at the inlet. You can keep the symmetry BCs on the left and right edges, and the fibers as stationary walls.

In my setup, the level of resin is going to rise through the fixed fibers. This is just a point-of-view (POV) perspective problem. What you seem to want is the POV of the resin surface; it sees the fibers descending. If you move your POV and sit on the fibers, you will see the resin surface rising up until you are below the surface. Perhaps instead of using one POV, which is difficult to simulate, you could use an equivalent POV which is easy to simulate. What kind of results are you trying to obtain and would they be the same values in either POV?

I haven't yet tackled a VOF model, but this seems like a good one to learn on, so I will be watching this discussion play out.


eufrat posted this 24 April 2018

Hi peteroznewman,

thank your for your input! I have thought about your approach before. 

So first of all, what is the purpose of this simulation? The purpose is to investigate the influence of parameters like velocity of the fibers diving in and time of them remaining in the resin on the amount of air, which gets captured in the resin. When modelizing such simulations, you want to be as close to reality as possible for obvious reasons. Therefore, I am not too comfortable with the approach of the fibers being stationary and the resin streaming in from below. I think that these two approaches would differ regarding the behaviour of the air. When the resin streams in from below, I imagine it to be easier for the air to being pushed just upwards.

But anyways, imagining is not knowing. Maybe I will have a try on this kind of approach to compare it with the other...




Raef.Kobeissi posted this 29 April 2018

I am not sure if I completely understand what you're after here, but if you want the fluid to flow sideways why don't you use the left and right all as outlets?


Raef Kobeissi

peteroznewman posted this 29 April 2018

Raef, I believe this is a two-fiber wide slice from a very wide array of fibers. The symmetry BCs on the left and right walls represent that case.

Eufrat describes wanting to study the velocity of movement of fibers into the fluid that is so high that air gets trapped between vertically aligned fibers because the viscosity (and surface tension?) is too large for the resin to have time to flow around the first fiber before the next fiber enters the fluid, trapping air between the fibers.

What do you think about the difference in results between lowering the fibers into the fluid versus flowing the fluid up through the fibers?  I thought the result would be identical, but perhaps not at velocities high enough to trap air behind a fiber. 


  • Liked by
  • eufrat
raul.raghav posted this 30 April 2018

Eufrat, this is 2D planar problem that you're dealing with. A symmetric BC assumes a zero flux across the symmetry boundary. Remember that there is zero convective flux (zero normal velocity) and zero diffusion flux (zero normal gradient of all the flow variables) across the symmetry boundary. When you consider VOF, there will be waves formed that'll try to move across the left and right boundaries. Therefore, the gradients of volume fraction or density would not be zero at the left and right boundaries. A translational periodic boundary condition would be something you might want to explore a bit more. I think periodic boundary conditions can be applied to the VOF model, but you might want to check that as well.

A youtube tutorial that might be of help to you for your simulation:

Ansys Fluent: Dynamic mesh


eufrat posted this 30 April 2018

Thank you for your answers.

Peter is right about the background of this simulation. The model is a tiny extract of the real situation, where countless fibers get impregnated together in a roving.

Also thank you, Rahul, for your tip regarding the Dynamic Mesh. I already had my time fighting with it, but by now it works pretty nicely.





raul.raghav posted this 30 April 2018

Eufrat, can you share a few details about how you ended up modeling your case? Like what boundary conditions you decided to use and what the results look like. Just curious .


peteroznewman posted this 30 April 2018

I liked Rahul's suggestion of a periodic BC. I don't use that in my Structural work, but it is very useful in CFD models. I am curious what you ended up using.


eufrat posted this 01 May 2018

Hi guys,

the Boundary Conditions are not my priority at the moment, so I have put this aspect aside for now. Currently I am working on my simulation to get it to finish the calculation process.

I have defined the motion of my rigid circles with a profile. The motion of the circles is of the following nature:

1. Translation from point A to B

2. A certain span of time without movement

3. Translation back from point B to A

I defined my time/place data in a way which represents a speed of the circles of 0.5 m/s.

The span of time without movement is about 5 seconds long with my current profile.

I tested the motion profile with the dynamic mesh preview, and it works fine. But i got some problems in the solving process. First of all, I use variable time stepping. While the cirlces move, it is necessary for the time step size to be 1e-6 seconds at max, otherwise I would get negative cell volumes because the mesh folds itself. When the circles have reached their point B, there is no further body motion for a time span of 5 seconds. During this time span, Fluent is free to use bigger time step sizes, which is totally fine and necessary for a acceptable solution time. 

Unfortunately, I have a problem regarding the transition (time-step-size-wise) from motion characteristic 2 to 3 I mentioned above. In phase 2 of my motion profile, Fluent uses bigger time step sizes up to 0.04. When motion characteristic 3 begins, which means that the circles move back from point B to point A with the same speed of 0.5 m/s, a much smaller time step (1e-6 s at max) is needed again, otherwise the simulation stops because of negative cell volumes.

So how do I make Fluent clear that on a certain point of time in the simulation, it needs to reduce the time step size to a certain value? Is this something which could be realized by a user defined time step or something? I will read about this topic anyway, because it seems the most promising feature regarding this problem at the moment, but it might not hurt to ask you guys about it either.