Learning Forum

[Weiqiang Liu]

hello all,

I am doing a catalytic combustion of methane in a straight planar channel. The gas mechanism is GRI 3.0 and the surface mechanism is Dutchman mechanism. 

I am using species transport and laminar finite rate model. In order to ignite the mixture, I patched a 2000k temperature to the whole computation domain and some combustion products like water and carbon dioxide in the rear part of the channel.

parallel mode of fluent is used with 8 nodes. after almost 170000 iterations of 4 days' computation, all the residuals are lower than 1e-4 though some fluctuations happen.

what confuses me is is the computation speed normal? or the computation should have converged much earlier? it doesn't because I did not set the model correctly. However, I am not really involved with the model setting too much. because it's a very simple and I built the model following the instruction of a tutorial.

since a lot of work has been published regarding to the similar case, I am wondering can anybody tell me is the iteration speed normal? or what is the right way to ignite the mixture?

the picture below shows the image of residuals. I have to say it's not beautiful at all.

[Rob]

Calculation speed is a function of physics, cell count, cpu clock speed, RAM & bus speed and number of cores. Given all of the variables there isn't really a "normal" speed! 

Spiked residuals like that tend to imply some transient features in the flow: I'd need to see the mesh and flow field to make any comments on that. 

Given it's a micro channel, how many cells have you across the width/depth of the channel?  

 

[Weiqiang Liu]

hello, 

the picture below shows the enlarged mesh.

the diameter of the channel is 0.5 mm. the thickness of the wall is 0.2 mm. the length of the channel is 20 mm. the overall cell number is 40000. my desktop has 8 cores with 8GB RAM. my CPU is AMD Ryzen 7 1700X Eight-core processor.

my case is steady-state. All the kinetics, thermo data and transport data are imported by chemkin files.

Thanks 

[DrAmine]

You can attach the mechanisms for your reactions so that other non ANSYS-Stuff can check if you want.

From my side have you checked the flux report for mass and energy if the case is really converged? Are you monitoring some global key parameters? Are they depicting a steady-state behavior.? Why am I asking: If I just look to the residual plot you shared it seems that the case is not converged (it seems). Which global setting and numerical method are you using?

[DrAmine]

Can you point us to the surface reaction mechanism reference?

[Weiqiang Liu]

I am not monitoring any global key parameters because I don't know what is the appropriate parameter to monitor. the mass flux between the inlet and outlet is balanced very early. should I monitor the outlet temperature or the energy flux of the outlet?

 

below you can find the surface mechanism:

https://www.detchem.com/mechanisms

 

thanks

[DrAmine]

You should monitor things like reaction rates, the concentration of some important species, the temperature of both cell zones (average, max value,..). The flux report for energy is also important. 

 

[Weiqiang Liu]

yes, I think flux report energy is important because the temperature keeps changing.

[DrAmine]

Yes but does it tell you that the run is converging?

[Weiqiang Liu]

no it's nor converging. the outlet temperature decreases all the way down from 2000K to 1400K. now it's still decreasing.

 

by the way, the species residuals keep fluctuating. Do you know some methods to help with the species residual convergence?

[DrAmine]

I would recommend playing a bit with URF's and/or use additional under-relaxation (coupled with pseudo transient).  On the other hand, I recommend checking ISAT and stiff chemistry solver for your detailed chemistry as this might accelerate your runs.

[Weiqiang Liu]

ok, I'll go and check it. thanks very much

[Weiqiang Liu]

hello, 

I just tuned the species and energy URF to 1. The temperature decreased dramatically . I would expect the maximum temperature will decrease to 300K after some iterations, in other words, ignition failed. 

I've tried a lot of methods to ignite the mixture. however, nothing succeed. do you know some methods to ignite the mixture in a species transport with laminar finite rate model?

weiqiang.

[DrAmine]

That is the only way which can be done in steady-state runs: patch a certain region where the species participating in the most fastest reaction with higher energy / temperature or to start with an equilibrium distribution or to use some other models which might fit as initialization (like non-premixed model). But as you do have wall reactions there is not other models which can be used as initialization. 

[Weiqiang Liu]

I once read a paper that ignition can be done to patch a 2000 k to the whole computation domain. however, the model in that paper did not include wall reaction. I am wondering is the ignition method different with and without wall reaction?

thanks very much

weiqiang

[Weiqiang Liu]

hello Amine,

can I ask you a question? somebody told me to remove the solid part of the computation domain and then give a fixed high temperature to the catalytic wall in order to ignite the mixture. 

I am now trying this method. However, I really can not understand the meaning of this method. I believe the wall temperature is calculated by CFD iteration. How can I know the temperature in advance. Besides, what if the calculated temperature is very different with the predefined wall temperature?

I can not imagine in a real combustion facility, the wall temperature can be known in advance?

weiqiang.

[DrAmine]

Either provide the spark or heat required to overcome the energy barrier for the reactions to occurs via patching a hot spot/zone or via providing non adiabatic walls.

[Weiqiang Liu]

providing non adiabatic walls? is it even easier to yield extinction?