Ok, that actually tells you a lot. Namely, that the problem is due to the multiphase models. The next thing to try is to reintroduce the multiphase models with the knowledge that there is some element of instability caused by them. I would use a homogeneous model since the phases should remain separate (correct?) and it's simpler.

Also, if you are not already using it, activate the coupled volume fraction option since this usually converges substantially better. This option is in Solver Control > Advanced Options > Multiphase Control > Volume Fraction Coupling. Select the option "Coupled". If you were using segregated before, this might actually solve your problem.

I should mention that even with the coupled volume fraction solver, you will probably have to use a smaller timestep as compared to the single phase case. Also, it was mentioned before, but be aware of your mesh quality. A relatively coarse mesh with good quality elements is a good place to start for debugging.

Well, using exactly the same setup as for single phase flow, including expert parameter and vf coupling, while decreasing timestep even at 10^-12 from 10^-6s keeps returning me this error in 1-2 tsteps:
Notice: The maximum Mach number is -----
.....
| ERROR #004100018 has occurred in subroutine FINMES.
| Message:
| Fatal overflow in linear solver

Before starting with 2 phase sim, i tried also to improve my mesh. Here it is:
http://img844.imageshack.us/img844/9674/immagine2ee.jpg
http://img844.imageshack.us/img844/6592/immaginezy.jpg

Any suggestion? Should i improve my mesh somewhere?

At the beginning of the run CFX reports some information about the mesh. Can you repost here? Looking at the surface mesh it looks okay, but maybe there are some bad elements in there somewhere causing problems. Also, make sure you are using first order advection for everything to start.

Also it is reporting Mach number, which means a fluid is compressible. Why is that required?

+--------------------------------------------------------------------+
| Mesh Statistics |
+--------------------------------------------------------------------+

Domain Name : Fluid

Total Number of Nodes = 328456

Total Number of Elements = 353071
Total Number of Tetrahedrons = 25845
Total Number of Prisms = 5924
Total Number of Hexahedrons = 267935
Total Number of Pyramids = 53367

Total Number of Faces = 74985

Domain Name : Porous

Total Number of Nodes = 105389

Total Number of Elements = 116186
Total Number of Tetrahedrons = 11037
Total Number of Prisms = 3763
Total Number of Hexahedrons = 76429
Total Number of Pyramids = 24957

Total Number of Faces = 42834

Global Statistics :

Global Number of Nodes = 433845

Global Number of Elements = 469257
Total Number of Tetrahedrons = 36882
Total Number of Prisms = 9687
Total Number of Hexahedrons = 344364
Total Number of Pyramids = 78324

Global Number of Faces = 117819

Domain Interface Name : Default Fluid Porous Interface

Discretization type = GGI
Intersection type = Topological

+--------------------------------------------------------------------+
| Vertex Based Partitioning |
+--------------------------------------------------------------------+

Partitioning of domain: Fluid

- Partitioning tool: MeTiS multilevel k-way algorithm
- Number of partitions: 4
- Number of graph-nodes: 328456
- Number of graph-edges: 2033214

Partitioning of domain: Porous

- Partitioning tool: MeTiS multilevel k-way algorithm
- Number of partitions: 4
- Number of graph-nodes: 105389
- Number of graph-edges: 659762

+--------------------------------------------------------------------+
| Partitioning Information |
+--------------------------------------------------------------------+

Partitioning information for domain: Fluid

+------------------+------------------------+-----------------+
| Elements | Vertices | Faces |
+------+------------------+------------------------+-----------------+
| Part | Number % | Number % %Ovlp | Number % |
+------+------------------+------------------------+-----------------+
| Full | 353071 | 328456 | 74985 |
+------+------------------+------------------------+-----------------+
| 1 | 99980 25.0 | 103177 25.2 19.8 | 28075 25.1 |
| 2 | 100833 25.2 | 102500 25.0 20.1 | 27873 24.9 |
| 3 | 98620 24.7 | 101179 24.7 19.9 | 27831 24.9 |
| 4 | 100637 25.2 | 103345 25.2 19.9 | 28106 25.1 |
+------+------------------+------------------------+-----------------+
| Sum | 400070 100.0 | 410201 100.0 19.9 | 111885 100.0 |
+------+------------------+------------------------+-----------------+

Partitioning information for domain: Porous

+------------------+------------------------+-----------------+
| Elements | Vertices | Faces |
+------+------------------+------------------------+-----------------+
| Part | Number % | Number % %Ovlp | Number % |
+------+------------------+------------------------+-----------------+
| Full | 116186 | 105389 | 42834 |
+------+------------------+------------------------+-----------------+
| 1 | 38123 24.9 | 44871 24.9 41.7 | 20180 24.9 |
| 2 | 38171 25.0 | 44985 24.9 41.0 | 20235 25.0 |
| 3 | 38431 25.1 | 45590 25.3 42.2 | 20382 25.2 |
| 4 | 38147 25.0 | 45037 25.0 41.4 | 20184 24.9 |
+------+------------------+------------------------+-----------------+
| Sum | 152872 100.0 | 180483 100.0 41.6 | 80981 100.0 |
+------+------------------+------------------------+-----------------+

First order advection means updwind scheme right?
If so i just set it up with no result.

@Ghorrocks
I don't want to be wrong, but guess compressible phase is needed to keep the fluid/porous pressure gradient...

I thought it would output some information on orthogonality and such as well. Anyways, your mesh has a fair number pyramids which usually are not very good quality. In which program did you make the mesh? In ICEM CFD you can get a histogram of a measure they call "quality". CFX recommends the quality is above 0.3 for all elements. Usually through smoothing you can get there. Try to check this metric and work on your mesh if it's low quality.

Running incompressible is fine for cases with porous media. I would recommend going that route since I am assuming your Mach number would be low enough.

Your use of compressible air (I presume it is air) could be the cause of some of these problems. Does the resin seep into the fibre bundles and compress the air into a region in the middle? This would mean the fibres do not fully wet and that sounds bad to me. I think it more likely that the resin seeps into the fibres and pushes the air along the fibre bundles to get it out of the way. This means the fibre bundles will fully wet. In this case you may also be able to use incompressibel air, but you will need to provide a mechanism for the air to escape.

You need to know these details and get them right before you have a hope of getting a simulation of it to work.

http://img833.imageshack.us/img833/2551/fibremesh.jpg
What i want you to know first, is that where we have air, it should be void instead. (this is why i do want the pressure to stay very low)
And the pic shows why i am not using an uncompressible air flow. The pressure gradient along the interface becomes null and this means very very small resin flow into porous media (recall darcy's law). I tried also to switch on surface force with a coeff = 1 N/m with no effect in keeping air.pressure way lower than resin's. (i choosed primary fluid = resin; is the coeff too low? - remember air = void for me)
Ghorrocks i'd expect air to make its way to porous.outlet without flowing into fluid domain (pressure here should be way higher) and with not much issues.

If i use exactly the same setup (compressible air) but with Resin's pressure closer to air's than this one, things go fine, i get convergence, i see what i do expect to see. As i run on higher pressures everything goes crap.

If there is a way to achieve pressure gradient using uncompressible flow it would be welcome, as i guess it helps convergence, right?

You have mentioned the pressure gradient many times, but never once mentioned where the pressure gradient comes from. Rather than trying to artifically create the pressure gradient you think is there, how about you model the conditions which make the pressure gradient come about - then the pressure gradient will form naturally.

I presume this fibre mat is in a pressure vessel into which resin is injected. What do they do in the pressure vessel to handle the air?

Ghorrocks, i'll try to do my best to make you understand the process with my poor English. Please, forget everything about this simulation before starting to read this.

Imagine you have a resin container which is at atmospheric pressure, let's call it 1. Then you have a fiber vessel, let's call it 2. At start, the valve connecting 1 to 2 is closed, so you have two separate environments.

A pump empties B of air and puts it under negative pressure. You have no more air, but vacuum instead. Then, you open the valve and let resin flow due to pressure gradient. Substantially, what i am trying to model using fluid = air is vacuum in truth. But Cfx has no way to model vacuum, and i think this is the best choice. We have small viscosity effects due to air, so the guess is to introduce very little error caused by this substitution. Again, in cfx i am setting up pressures different from the physics, in which we have like 0Pa at inlet and -10kpa at outlet; infact i am using 10kpa at inlet and 0kpa at outlet. Basically i don't think to introduce any issue with this, since what really matters is pressure gradient and not pressure itself.

Moreover, we start with Resin volume fraction = 1 in the fluid domain because we can assume fiber impregnation starts only after the elementary cell (fluid domain) is already filled; this is because resin flow in fluid domain should be way faster than fiber impregnation, and so our assumption should introduce a very little error, again.

Of course, pressure gradient along flow direction will not be fixed for every elementary cell and in time, so i'll need to make different simulations with different outlet pressures/inlet mass flows.

I hope to have been clear.
Sorry again for my English.

Your English is very clear, I understand what you are saying. Some important points:
* You do not have a vacuum. You have air under a low pressure. There is still air in the fibre reservoir, just not much - but the air which is there is important.
* CFX cannot model a vacuum because they don't exist :) At least not in the Navier Stokes world anyway.
* So this should be modelled as air at whatever pressure it is at.
* I disagree that the absolute pressure is not important. The absolute pressure sets the air density and therefore the trapped air mass. This is critical, so you must set the absolute pressure level correctly.

I think the convergence problems youare having is because you are not modelling the resin flow into the fibre chamber correctly. You seem to be missing some important points. Another key point you have not discussed is whether the vacuum chamber keeps appying a vacuum as the resin enters, or whether it is sealed. And do you keep the vacuum on until you pull resin out the other side to ensure the fibres are fully wet? These types of details affect the way you should model it.

Sorry for this absence.
Finally i think i solved my problem. Since i had never used ICEM before, i had to give a look into tutorials et cetera.
When my simulations diverged, i noticed everything started in a little region in which pressure values growed like crazy. That was due to low quality elements. Now Everything looks fine thanks to some working in ICEM.
Thank you really for your help. Again.