[willsen]

Hi Everyone!

I am trying to model resin flow through a textile unit cell as can be referred to the attached picture. From the picture, it can be seen that there will flow through the inter-tow channel (the gap BETWEEN the fibrous tows) and intra-tow channel (INSIDE the fibrous tows as each fibrous tow consists of thousands of fiber filaments).

To model the flow through this unit cell two domains shall be defined: fluid domain (inter-tow channel) and porous domain (intra-tow channel).

The way I would like to approach this is by first calculating the permeability tensor inside the tows through an analytical equation (which I have already calculated from the information of the porosity inside the tows and the fibre radius).

To model the flow inside the tows, I would like to input this permeability tensor inside the tows (with appropriate matrix transformation) depending on the principal direction of the tows and obtain the velocity inside the tows in term of superficial velocity. So I don't really need to input this porosity information to ANSYS CFX as it has already been taken into account when I calculated the tows' permeability analytically.

To my understanding, ANSYS CFX allows me to obtain this superficial velocity field inside the tows by simply adding momentum loss term to the governing flow equation (without altering the equations like in the full porous model). According to the documentation (I screenshot the relevant section from Solver Theory Guide), this is done by defining the porous body as FLUID DOMAIN. However, ANSYS CFX only allows me to add these directional momentum loss terms in the POROUS DOMAIN under the porosity setting tab. Is there a miscommunication from the documentation?

Furthermore, the momentum loss term requires both PERMEABILITY and QUADRATIC LOSS COEFFICIENT. How do we calculate this quadratic loss coefficient? I have never come across any literature in the field of textile permeability that includes this quadratic loss coefficient in their numerical model.

Thank you very much everyone!

[siw]

You can use a fluid domain rather than a porous domain for the directional momentum loss terms, but the porosity parameter is not included this way.

I have never found a way to calculate the quadratic loss coefficient. Instead I have had to calculate the permeability and quadratic loss coefficient solely from experimental data; i.e. vol. flow rate vs pressure loss curve across the filter media of interest. Your flow must be laminar so not surprising you have not found this in the literature as this extra term (a velocity squared term) is negligible and you only need the permeability.

[willsen]

Hello Stuart!

Really appreciate your kind advice on this. Yes, I just realized that the quadratic loss coefficient term can be neglected in my case as it is a type of creeping flow.

I have gone through the ANSYS CFX documentations in more depth. Please correct me if I am wrong:
ANSYS CFX allows to 2 ways to model flow through porous media:
1. Superficial velocity formulation, which is defined in a sub-domain of a fluid domain. The momentum loss term will take into account the effect of porosity thus the governing equations are not modified at all. The velocity field obtained from this formulation is superficial velocity field instead of true velocity.

2. True velocity formulation/full porous model, which is defined in a porous domain. The porosity will modify the governing equations. Thus, the velocity field obtained from this formulation is the true velocity field. With this formulation, the defined loss coefficients can either be derived from true velocity or superficial velocity.

If my understanding is correct, which of the formulation will be more accurate? As I am only interested with the mass flow rate through my textile unit cell, will both formulations give me the same mass flow rate result?


Do you think I can contact you directly you through your email? Thank you very much!

[siw]

Your two points are summarized in the CFX v17.2 Theory Guide Section 1.12.

I use the fluid domain with directional momentum loss terms when I model filters in a large systems because I just want the pressure loss to be correct, so my filters are "black boxes" in the type of models I work on. However, it seems you are modeling a local portion of a filter, your textile unit cell. So I am unsure why you are even considering porous flow modelling and not just a regular low Reynolds number flow where the fibres are walls (maybe rough walls) with inlets/outlets or periodic boundaries.

Rather than contact someone directly it is better to post here then you get a wider audience and more people can help.

[willsen]

Thank you Stuart. Appreciate your help!