[J_Keel]

Hello everyone,

I'd like to thank you in advance for taking the time to read my post, I've worked on this problem for some time now and am in great need of assistance.

I am trying to model steady state ionic reactions (rate constants ~1e-10 [s^(-1)]) in a T-mixer under laminar flow conditions (average residence time ~0.5 [s]). The simulation is stable when I use a physical timescale of around 1e-6 [s] but instabilities in the source terms arise when I increase this. I have tried using a local timescale factor of 2, this stabilises the source terms and leads to convergence, but when switching back to a physical timescale to finish off the run the maximum physical timescale which is stable is once again of the order of 1e-6 [s].

It is clear that I cannot run the whole simulation to convergence using such a small timescale. I came across the following in FLUENT documentation and wondered whether CFX had similar capabilities:

A second convergence issue in reacting flows involves the magnitude of the reaction source term. When the FLUENT model involves very rapid reaction rates (reaction time scales are much faster than convection and diffusion time scales), the solution of the species transport equations becomes numerically difficult. Such systems are termed "stiff'' systems. Stiff systems with laminar chemistry can be solved using either the pressure-based solver with the Stiff Chemistry Solver option enabled, or the density-based solver (see Section 14.1.7).

SOURCE: http://aerojet.engr.ucdavis.edu/flue...ug/node608.htm

Once again thank you very much for your time!

Jamie

Edit: If CFX has no in-built function to reduce the stiffness of the reaction source terms, do you think it is possible, through expressions, to implement the following into CFX:

SOURCE: http://aerojet.engr.ucdavis.edu/flue...chem-seg-rrate

[Opaque]

There is a mechanism for dealing with stiff chemical reactions in ANSYS CFX, but it is an expert setting. You should contact ANSYS support for more information.

In the meantime, have you tried relaxing the material component (species in FLUENT speak) that may be causing the problem ? You can do that by adding a dummy source term, i.e. zero source and non-zero source coefficient.

[J_Keel]

Hi Opaque,

Thank you very much for your response.

Originally Posted by Opaque

There is a mechanism for dealing with stiff chemical reactions in ANSYS CFX, but it is an expert setting. You should contact ANSYS support for more information.

OK, I shall contact them.

Originally Posted by Opaque

In the meantime, have you tried relaxing the material component (species in FLUENT speak) that may be causing the problem ? You can do that by adding a dummy source term, i.e. zero source and non-zero source coefficient.

The reaction scheme is as follows:

(1) A + B -> R
(2) D + E + B -> S
(3) S + D <=> Q

The main reaction causing the stiffness is reaction (3). In a sub-domain, I have written the source terms for all components by summing them across all reactions; and the source coefficients as the component source term's partial derivatives.

Where exactly will I place this dummy source? Will I need to create an additional sub-domain? Or would multiplying the source coefficient's for S, Q and D by a factor be the equivalent?

Thank you for your time!
Jamie

[Opaque]

You are creating the source terms manually ? How come ? can you not use the provided functionality to describe the reactions rate you are trying to model ? Then, the software deals with them directly.

If you are adding the source terms manually, you must also deal with the numerical details of robust source term linearization and mass fraction bounding, i.e. never allow the mass fraction to get out of bounds w/o clipping the solution values. Have you check the Combustion Source Term Linerization section of the documentation.

On the subdoman approach earlier, you do not need another sub-domain but only scale the existing source term coefficient.

[J_Keel]

Originally Posted by Opaque

You are creating the source terms manually ? How come ? can you not use the provided functionality to describe the reactions rate you are trying to model ? Then, the software deals with them directly.

Thanks once again for your reply.

When I started this project I was completely new to CFX and hence I inputted the source terms manually with expressions as I was sure of their mathematical formulation as opposed to using a 'black box' I wasn't confident with. I have tried using the reaction function and noticed no difference in rate of convergence or stability, so I assumed the source terms from the reaction function are treated with the same algorithm as sources created from a sub-domain - is this not the case?

Originally Posted by Opaque

On the subdoman approach earlier, you do not need another sub-domain but only scale the existing source term coefficient.

I've multiplied the source term coefficients by a factor of 5 and managed to ramp up my timescale by the same factor without causing instabilities. Hopefully I can keep doing this until I get close to the advection timescale. Thank you for your solution.

--------------------------------------------------------------------
(These are not issues I'm facing, I just thought they'd be interesting discussion.)

Originally Posted by Opaque

If you are adding the source terms manually, you must also deal with the numerical details of robust source term linearization and mass fraction bounding, i.e. never allow the mass fraction to get out of bounds w/o clipping the solution values. Have you check the Combustion Source Term Linerization section of the documentation.

I have finished reading the 'Combustion Source Term Linerization' section. It is a very elegant way of stabilising the source terms but unlike Picard's method where the source term coefficients can be manipulated without affecting the actual magnitude of the source terms, here it seems the actual source terms are being tampered with. Does this not have an affect on the solution?

SOURCE: http://www.arc.vt.edu/ansys_help/cfx_thry/i1309497.html