Assigning intra-tow permeability to tows within ANSYS CFX

[willsenwijaya]

Hi Everyone!

After generating a textile unit cell in TexGen, I am planning to run a flow simulation in ANSYS CFX by using this unit cell. To model the flow within the tows, ANSYS CFX can do this by requiring us to input the intra-tow permeabilities along with its principal/stream-wise direction. However, the specification of this intra-tow permeability can only be done per sub-volumes of the analyzed geometry. My question is that:
1. Is there a way that we can make the local coordinate system of the tow elements to be aligned with its principal direction (the direction of the tow path)?
2. Has anybody ever tried to do the same thing in ANSYS CFX and can recommend the more efficient way to assign the intra-tow permeabilities to each of the tow elements according to their principal direction?


Thank you in advance.

[louisepb]

Hi,

My colleague Xuesen has given the following response (as this is definitely not my field of expertise!):

You may refer to CFX user manual on Coordinate Frames in the CFX-Pre User's Guide https://www.sharcnet.ca/Software/Ansys/ ... 07828.html. It allows you to define local coordinate systems by CEL expressions.

More importantly, I would like to highlight the limit with CFX to predict permeability.

For a typical textile reinforcement with permeability > 1 x 10-12 m2, the CFD analysis can neglect the effects of porous tow.

To implement the porous tow in CFX, there is a numerical problem with CFX setup. CFX only uses Darcy’s equation in the porous domain. As a result, it does not ensure the continuity of shear stress at the interface of pure fluid domain and porous domain. For permeability prediction at order of 1 x 10-12 m2, CFX would over predict the permeability by 20-25%. In theory, the Brinkman equation shall be used, instead of Darcy’s equation. However, there is serious convergence issue with Brinkman equation.

This problem may outweigh the benefit of defining orthotropic permeability tensor and including porous tow.

Hope that helps,
Louise

[willsenwijaya]

Hi Louise,

I am really grateful for your kind reply! To my understanding, CFX allows you to model flow through porous media by using two methods: superficial velocity formulation and true velocity formulation.
The method that I am planning to adopt is the superficial velocity formulation, which is basically the laminar Navier-Stokes equation with additional source term. This source term is referred to as the momentum loss model which will take into account of the viscous losses through permeability. I am not sure if this formulation is equivalent to the Darcy's law? By chance do you have the resources that explain about the limitation of ANSYS CFX just like what you explained to me?
Once again, thank you very much!

[louisepb]

Hi,

Xuesen replies as follows:
In CFX, the interface issue will be the same for either superficial velocity formulation or true velocity formulation. It comes into light, through the ANSYS technical support. I do not have any publication on this matter specifically related to ANSYS CFX. I would suggest to run a simple test case in CFX, such as a single flow channel bounded by porous fibre tows.

Hope that helps,
Louise

[willsenwijaya]

Thank you very much! I shall investigate this further. Appreciate the advice