[siw]

Hi,

I am modelling a filter as a fluid subdomain within a larger system using the directional loss components, permeability (Kperm) and loss coefficient (Kloss), where the Kperm and Kloss where obtained from an experimental filter pressure drop vs volumetric flow rate polynomial curve fit all based on the superficial velocity. I do not need to model the filter internals (far too complex) and I am only interested features such as pressure drop etc. on the system, which the filter is within.

However, I want to include sink terms for the SST k and omega equations because the real filter has wire meshes on its inlet and outlet (also the filter contents is small pathways) there no upstream turbulence can pass through the filter to the downstream and no turbulence will be generated inside the filter. The pressure drop contribution of the wire meshes is accounted for within the experimental data.


For this I made an Expression for each the k and omega equations and for a source coefficient as follows:

TKE Sink = -(Density*Turbulence Kinetic Energy)/(Physical Timescale*Courant Number)
TEF Sink = -(Density*Turbulence Eddy Frequency)/(Physical Timescale*Courant Number)
Source Coeff = -Density/(Physical Timescale*Courant Number)

since the units are consistent. However, the simulations with and without the sink terms gave the same results in CFD-Post when I checked contours of pressure, velocity, eddy viscosity ratio, turbulence kinetic energy and turbulence eddy frequency.

Anyone have any ideas on suppressing upstream turbulence inside a subdomain and not producing new turbulence in a subdomain?


Thanks.

[ghorrocks]

You appear to be trying to model the source term as proportional to TKE (for the TKE equation). What physical justification do you have for this?

Also, why is the denominator Physical Timescale*Courant Number? What is the physical justification for that? This would make your source term dependent on the time step size of the simulation - this does not sound physically correct to me. Should it be something like the residence time in the subdomain (distance/velocity, where distance is the thickness of the filter, velocity is the velocity of the fluid perpendicular to the filter membrane)?

Or should you just set the TKE to zero on the downstream side of the filter?

[siw]

Thanks Glenn, was hoping you'd reply to this thread.

I was in contact with ANSYS technical support when I first started looking into this and they proposed the TKE and TEF sinks and source coefficient equations. However, recently ANSYS have transfered our commerical account to a Channel Partner, so I no longer get direct ANSYS contact and the Channel Partner support is very lacking.

How can I set the TKE to zero as you say? As far as I can see this is only possible using an expression in the subdomain TKE equation source input. I do not see any other options available, such as locally switch off the turbulence.

[siw]

Further thoughts.


I tried with a very high (negative) number for the equation source TKE but that caused convergence difficulties and the contour plots of velocity, TKE etc. where adversly affected in the fluid upstream of the filter subdomain, even though the sink is only applied to the subdomain.

However, the TEK sink expression looks the same as the unsteady term in the k-equation . Since my simulation is steady-state then that is why it is not having any effect.

Therefore, perhaps the TEK sink expression must be a negative of the advection term in the k-equation i.e. . However, I cannot make an expression with a product of divergence operator terms, only single parameter gradient is allowed e.g. Velocity u.Gradent X

[ghorrocks]

It is simple to set a variable to a value with a source term. Have a look at the CFX-Solver Modeling Guide, section 1.3.2.2.2.

Your desired TKE value is zero, so k(spec) = 0. Then the source term is -C*(k-k(spec)) which simplifies to -C*k. You then use a source term coefficient of -C. Make sure C is large enough to pull it to zero quickly, but small enough to not cause convergence problems.

This approach is simple and reliable. I have used it many times.

Note that I would not apply this term to omega. Unless you know what an appropriate value for omega is I would leave it untouched. An even better approach would be to do a sensitivity study on omega to see if the value for omega here makes any difference. If it does make a difference then you will have to have a think about an appropriate value for it.

[siw]

Thanks for replying Glenn.

Just to recap so that I understand correctly after reading your message and the part of the User Guide you referenced. I should make the following two expressions:

Sink Coeff = -10^5 [kg m^-3 s^-1]
TKE Sink = Sink Coeff * Turbulence Kinetic Energy

I start with -10^5 as it is large and pinched from the User Guide.

[ghorrocks]

Yes, that is correct. You may need to adjust 10^5, but based on typical values of k it should be OK.

[Opaque]

Let take a hypothetical case of a non-porous domain followed by a porous domain.

Where doe the turbulence generated in the first domain goes when it crosses the interface? Does it just disappear, or gets advected w/o further generation/dissipation?

You can also set the Eddy Viscosity = 0 for the porous domain only (Turbulence Model/Advanced Settings), and the turbulence upstream will be advected only since every other term will be exactly 0, correct?

[siw]

Thanks Glenn.

Using the -C(k-kspec) with C = 10E5 worked well and looked intuitive in CFD-Post. A simple resolution in the end.

I assume the turbulence scales that are too large to enter (and pass thorough) the porous domain are terminated and their energy is wasted as heat, as my situation is low speed then the heat might trivial - but I am cannot confirm. But I makes sense that due to the filter's wire gauze and small internal pathways that the energy from the larger scales cannot pass through or develop inside the filter. No doubt PhD's have researched this (I would too if I was concerned about the flow just of the filter alone) but for my industrial case what I have used for assumptions for a large flow system is suitable. No wanting a discussion about turbulence in filters this thread has answered my CFD query - thanks.

[ghorrocks]

Risking incurring your wrath here....

The flow in the small passages in the filter have low Reynolds number. Low Reynolds number flows dissipates turbulence, especially if it is below the turbulence transition Reynolds Number.