[stefdc]

Hi everybody,

I created a new material called flue gas where the properties varie with the value of the temperature. I used the piecewise-linear. I ran a steady state simulation in order to initialize the values. The problem is that if I disable the energy equation, the solution converges, but when I turn on the energy equation I get the divergence message.

Do you have any idea? What should I do?

thanks

[LuckyTran]

If you disable the energy equation of course it can't diverge. This problem is too general to give a definitive answer to. Make sure you have a good initial guess.

Which properties were have the temperature dependence? Try using a lower URF for the affected equations.

Try enabling the energy equation in the models but disabling the energy solver in solution controls. This helps to update the current property field so it is consistent with the newly defined properties. After a few iterations (30 or so), enable the solution of the energy equation.

[stefdc]

Originally Posted by LuckyTran

If you disable the energy equation of course it can't diverge. This problem is too general to give a definitive answer to. Make sure you have a good initial guess.

Which properties were have the temperature dependence? Try using a lower URF for the affected equations.

Try enabling the energy equation in the models but disabling the energy solver in solution controls. This helps to update the current property field so it is consistent with the newly defined properties. After a few iterations (30 or so), enable the solution of the energy equation.

Thanks a lot for your answer. My material is a fluid with the density, cp, and viscosity, function of the temperature. I have a furnace at 1500K with inside the flue gas and outside I created an enclosure with air at ambient temperature. I created a door and I used a profile in order to simulate the opening of the door. I want to evaluate the behavior of the furnace during the opening. I already did a simulation like this, but I supposed air at 1500 K inside the furnace instead of flue gas. The precedent simulation converge at every time step. For this new one I enabled the energy equation in the models and I disabled the energy solver. When I turn on the energy solver the simulation diverges. I tried to modify the URF but nothing. I think the problems are with the new material because is the only thing I changed.

If I disable the energy solver in solution control, can I get information about the convective heat flux during the opening? I use flow rate--temperature--entalphy to evaluate the flux.

thanks!

[vasava]

Originally Posted by stefdc

I have a furnace at 1500K..........

I recommend you double check your material properties and verify that they are valid for this temperature.

Next, you can plot temperature contours and have a close look at region where temperature distribution is abnormal. If you have coarse or poor quality mesh, you may need to refine your mesh.

Read errors and warning in the command window carefully. If you have a warning about limited temperature, you may need to lower your time-step, refine mesh, consider changing relaxation factors and use better discretization scheme (either all or some of these).

If you post output printed in the command window as well as some pictures of the mesh and results, would help determine the problem with your simulation.

[LuckyTran]

You need to ease the simulation into accepting the wildly different material properties. Highly non-linear simulations require more care than mildly non-linear ones.

[stefdc]

Thank you again!!! You were very kind. Here some pics of my simulation.

First of all I tried to initialize the solution with a steady state simulation and then swicth into a transient simulation with a time step of 0.1 s for 410 time step (total time of the opening 40 s).

I checked several times the values inserted for the flue gas and they were correct.

I tried to implement the simulation with a SIMPLE method and I got this message (it is the im2.jpg):

Error: Divergence detected in AMG solver: pressure correction

Error: Divergence detected in AMG solver: pressure correction
Error Object: #f

the same thing happens if I use the COUPLED Scheme but with the message:

Error: Divergence detected in AMG solver: Temperature

I really don't know what to do.

Do you think that the assumption of air inside the chamber instead of flue gas can be accepted?

I have another question. My furnace works with an over pressure of about 40 Pa, I set the operating pressure at 101325 Pa in operating condition and then, after the initialization, I patched the Pressure of the furnace at 101360 Pa and the air at 101325 Pa. Is it correct or should I modify it?
I have no inlet or outlet in my domain, just walls.

[Kosmosisy]

If you have data table for your fluid, try to fit a at least third or fourth order curve. Use this function with polynomial model not piecewise. In addition, make sure your data table covers all possible temperature range in your simulation. For example, lets say that your maximum temperature data point is at 1000K, but your simulation goes to 1500K. If it happened, your simulation would diverge. In addition, you could easily fit a curve with excel.

[stefdc]

And here we are. I've just enabled the energy solver.

[stefdc]

Originally Posted by Kosmosisy

If you have data table for your fluid, try to fit a at least third or fourth order curve. Use this function with polynomial model not piecewise. In addition, make sure your data table covers all possible temperature range in your simulation. For example, lets say that your maximum temperature data point is at 1000K, but your simulation goes to 1500K. If it happened, your simulation would diverge. In addition, you could easily fit a curve with excel.

Thank you!! I'll try to use a polynomial, I've never tried it but it should be easy. I'll let you know!!

[stefdc]

I've tried but it still doesn't work. I used a piecewise polynomial. The dependence of the viscosity with the temperature is an hyperbole.

[Kosmosisy]

Originally Posted by stefdc

I've tried but it still doesn't work. I used a piecewise polynomial. The dependence of the viscosity with the temperature is an hyperbole.

Use only polynomial, not piecewise linear or piecewise polynomial. However, run your case with constant parameters first and then see what happens. Next, try to use "polynomial" values except viscosity, for the viscosity lets assume it as constant again. Moreover, could you please post your "operating conditions" section.

[stefdc]

Originally Posted by Kosmosisy

Use only polynomial, not piecewise linear or piecewise polynomial. However, run your case with constant parameters first and then see what happens. Next, try to use "polynomial" values except viscosity, for the viscosity lets assume it as constant again. Moreover, could you please post your "operating conditions" section.

My first simulation was with constant values (air) and it was good, it converged every time step. Now I would like to know how the convective heat flux changes if I use flue gas instead of air.

I can try with a constant viscosity and a polynomial. I attached a pics of some of my properties.

Now is converging, but just because I disabled the energy solver.

[Kosmosisy]

Originally Posted by stefdc

My first simulation was with constant values (air) and it was good, it converged every time step. Now I would like to know how the convective heat flux changes if I use flue gas instead of air.

I can try with a constant viscosity and a polynomial. I attached a pics of some of my properties.

Now is converging, but just because I disabled the energy solver.

Why is the thermal conductivity of flue gas equals zero? It is not physical. When you activate the energy equation FLUENT does calculate Nusselt number. In your case, your Nusselt number goes to infinity and then Reynolds also goes infinity because of that. You could see from your one of posted picture. Your flow rate goes to infinity, because in Reynolds number, all the parameter are constant or have range except velocity then FLUENT try to calculate infinite velocity.

[LuckyTran]

In Fluent, pressures are in gauge pressures. If you patched a value of 101360 & 101325 then both of those would be at an absolute pressure of ~2atm.

Originally Posted by Kosmosisy

Why is the thermal conductivity of flue gas equals zero? It is not physical. When you activate the energy equation FLUENT does calculate Nusselt number. In your case, your Nusselt number goes to infinity and then Reynolds also goes infinity because of that. You could see from your one of posted picture. Your flow rate goes to infinity, because in Reynolds number, all the parameter are constant or have range except velocity then FLUENT try to calculate infinite velocity.

Zero conductivity does not cause this infinite velocity result. Nusselt number and Reynolds number are purely post-processing values, they do not affect the solution. Fluent doesn't calculate velocity from Reynolds number.

[stefdc]

Thank you for your time! I think that for the knowledge of the convective heat flux my results can be considered reliable, even if I disabled the energy solver. What do you think? I attached the flow rate obtained.

[stefdc]

Just a little update!!! My simulation is converging, I modified the properties of the air. In the precedent simulations I used constant parameters and the ideal gas law for density. Now I inserted a piecewise linear for all the properties and is converging with the energy solver turned on!!! I'm happy!!!!

[Oula]

Originally Posted by stefdc

Just a little update!!! My simulation is converging, I modified the properties of the air. In the precedent simulations I used constant parameters and the ideal gas law for density. Now I inserted a piecewise linear for all the properties and is converging with the energy solver turned on!!! I'm happy!!!!

I very much like when people share their experience in solving the problems that they had with their work and how they solve it. This is really useful for future visitors, you could save someone's future (and life ) with just few words. Thanks Stefania