Moving porous media problem
 

Hello everyone,

I am using CFX to simulate resin flow into fibre stack in the chamber of an impregnation die. There are two domains and three boundaries in this model. Details can be seen in the attached file. There is an interface between liquid domain and porous domain. The problem I am facing now is that the resin doesn't flow into the fibre stack through the whole interface. Instead, the resin flows to the fibre inlet and penetrate fibre because of the negative pressure in this area.

My questions are: why I got negative pressure in the results? Why can't the resin flow into the fibre stack through the whole interface between liquid domain and porous domain?

I would really appreciate if anybody can help me with these questions.

Regards,

Jerry

Negative pressure just means the pressure is below your reference pressure. There is nothing wrong with this - but negative absolute pressure needs some thought to consider whether the results are physically realistic. There are only a very small number of circumstances in CFD when negative absolute pressure is correct, most of the time it means you have a modelling error.

I do not understand your comments that the resin does not enter the fibre stack. You would need to show an image of what you are getting and what you expect for us to understand what you are talking about.

A final point: Please just post images directly on the forum. Do not attach them as word documents.

Hi Glenn,

Thanks for your support.

In this model, the fiber stack is treated as a porous media. The resin flow will obey Darcy's law to penetrate the fiber stack in both longitudinal and transverse direction. Since the fiber stack is moving, resin will be pulled by the fiber once the resin flows into the fiber through thickness direction. The original pressure in the porous domain is atmospheric pressure and injection pressure is 2 atm. So this pressure gradient will force the resin to flow into the fiber stack through thickness direction. The time for the resin to penetrate the fiber stack through thickness direction is determined by the chamber length and pulling speed. The transverse velocity of resin is extremely low due to low transverse permeability. Therefore, the thickness of the wet fiber stack should increase gradually along the pulling direction.

In my simulation results, the resin can penetrate the fiber stack through thickness direction with relative high velocity because of the negative pressure which generate high pressure gradient in that area. So resin thoroughly penetrate the fiber through thickness direction within short time then it is pulled by the fiber to the outlet.

I expect the dry fiber stack comes into the die from fiber inlet and it is wet out by resin gradually. Resin flows into the fiber stack through the whole domain interface. The pressure in dry fiber area should be atmospheric pressure. I drafted the expected flow field and attached it here.

I would really appreciate if you can give me some advice.

Regards,
Wu

Why have you got an interface between the fibre/porous region and the resin region? These should be a single domain with the porous region being a sub-domain. Then you don't need an interface.

I am not sure what you question is, but if you are asking why isn't the pressure in the dry fibre area not atmospheric pressure - then that suggests you have set the simulation up wrong, probably in the boundary conditions. If you want us to help you you will need to post an image showing where your boundary conditions are located and your output file.

Hi Glenn,

In my model, the porous region is moving from fiber inlet to the taper while the liquid region is static. I want to track the flow front in the porous region to see how deep the liquid can penetrate the fiber through thickness within a certain time.

Should I use transient simulation to solve this problem? Do I need to apply dynamic mesh or momentum source to simulate the motion of fiber stack?

Thanks,
Jerry

I don't understand why your first sentence is relevant. Is that your justification of why you have an interface? If so then it does not make sense, and the interface is not required. The porous region can be implemented without an interface.

Should this be transient? I don't know the details of what you are trying to model so I cannot tell. I suspect this reaches a steady state condition after the initial transient is completed but only you know whether that is important or not.

If I was doing this I would probably not use the built-in porous model at all, but I would use a momentum source term as you can then impose whatever resistance you like, and can make it move at whatever velocity you like, and it can be done on a single mesh (no interface) with no moving mesh. But note I would not call any multiphase model "simple".

Hi Glenn,

Thanks for your prompt reply. I understand what you are talking about the interface. But CFX will generate an interface automatically when I create a subdomain for porous media in liquid domain. I am not sure if that interface the one you referred to.

What I am simulating is the flow model of a resin injection pultrusion process. Fiber stack continuously enters into an impregnation die, in which the fiber will be wet out by the resin in the chamber (see the attached picture). A positive pressure is applied on the inlet, resin will have the same speed as that of moving fiber stack on the outlet. The fiber inlet boundary condition is set as symmetry because fiber enter the die from there, no resin flow into die from this fiber entrance. I applied momentum source to account for the moving porous media.

The problem is that I didn't get the expected flow field as shown in the attached result picture. The simulation results I got are shown in the attached pictures (result 1 & 2). Negative pressure exists inside the die close to fiber entrance. All the resin flow into the fiber stack from that area because of the negative pressure. I changed the boundary condition to opening for fiber inlet, then the resin come into the die through fiber inlet from outside, which is not expected in my case. I also tried outlet boundary condition with atmospheric pressure for fiber inlet, negative pressure cannot be eliminated in that area.

The aim of doing this simulation is to find out the how much fiber can be wet out within the die.

I would really appreciate if you can give me some advice on this problem.

Regards,
Jerry

Please post your output file.

Hi Glenn,

I attached the output files. Please take a look at them.

Thanks,
Jerry

No, that is not what I meant. The output file is the text file which logs the progress of the run as it progresses. It will have the extension *.out.

Hi Glenn,

Is this the right file you are after?

Regards,
Jerry

That is the correct file, thanks. Now I can see exactly what you are doing.

You are modelling the resin as single phase. From your description I thought you intended to track the penetration of the resin into the fibre bundle as it displaces air. This sounds like a free surface multiphase model to me. Have a look at the CFX tutorial examples for how to set up free surface models - the relevant example is "Free surface flow over a bump".

Changing to a free surface model is going to fundamentally change the setup and the results you get. Not much point looking any further into your model if the fundamental approach does not appear correct.

Thank you very much, Glenn. I am working on a multiphase model now. I started with a simple geometry. The result is not bad. Thanks again for your help.