[cgswjs]

Hello everyone,
I've been doing this heat exchanger simulation for months and I tried out different turbulent models, solvers and mesh sets. The temperature profile updates when I use steady solver but the results are not very accurate compare to my benchmark values. So I tried to use the implicit unsteady solver to see if it gives me a better result. However, the temperature magnitude contour doesn't update when I use the unsteady solver. Same mesh set was used as I used steady solver. Can someone help me to resolve this issue? What could be the reason that causes this problem?

[flotus1]

Time step size too small? Steady state reached already?

[cgswjs]

Originally Posted by flotus1

Time step size too small? Steady state reached already?

If I can get a reasonable result from steady solver does that mean this is a steady case? I’m using 0.001 for time step right now. I will try larger ones to see if it works

[flotus1]

If I can get a reasonable result from steady solver does that mean this is a steady case?

Either that, or the time step size is just so large that any unsteadiness that might be present gets smoothed out.

For choosing a suitable time step size, you need an estimate of the time scale of the unsteady effects you expect to occur. Otherwise, you are just taking shots in the dark.

[cgswjs]

Originally Posted by flotus1

Either that, or the time step size is just so large that any unsteadiness that might be present gets smoothed out.

For choosing a suitable time step size, you need an estimate of the time scale of the unsteady effects you expect to occur. Otherwise, you are just taking shots in the dark.

Thank you.

[cgswjs]

Originally Posted by flotus1

Either that, or the time step size is just so large that any unsteadiness that might be present gets smoothed out.

For choosing a suitable time step size, you need an estimate of the time scale of the unsteady effects you expect to occur. Otherwise, you are just taking shots in the dark.

Hi there, I have one more question about the unsteady solver. Is it possible that the fluid flow is unsteady but the thermal properties are steady? It seems unsteady solver gives better flow results but won't update the temperature while steady solver updates temperature correctly with poorer velocity magnitude contour. Thank you.

[flotus1]

You might be dealing with conjugate heat transfer. Hard to tell from the information at hand.

[cgswjs]

Originally Posted by flotus1

You might be dealing with conjugate heat transfer. Hard to tell from the information at hand.

Yes I am doing a simulation for heat exchanger involves heat transfer from solid to fluid. Does this kind of simulation need special treatment to achieve a good result?

[arjun]

Originally Posted by cgswjs

Yes I am doing a simulation for heat exchanger involves heat transfer from solid to fluid. Does this kind of simulation need special treatment to achieve a good result?

What software are you using. Your solver is using implicit under-relaxation and the value of it might be low. In the solid regions it should be very high around 0.95 to 0.99 etc.



Set the energy urf to 0.99 and check.


PS: This is why in Wildkatze solver in solids the urf is set to 1 and a separate explicit urf is used to update the temperature.

[cgswjs]

Originally Posted by arjun

What software are you using. Your solver is using implicit under-relaxation and the value of it might be low. In the solid regions it should be very high around 0.95 to 0.99 etc.



Set the energy urf to 0.99 and check.


PS: This is why in Wildkatze solver in solids the urf is set to 1 and a separate explicit urf is used to update the temperature.

I am using Star CCM+ and I didn't change any URF values. I will try it out. Thank you

[arjun]

Originally Posted by cgswjs

I am using Star CCM+ and I didn't change any URF values. I will try it out. Thank you

Starccm has dual under-relaxation and you can set high urf for solids and lower explicit urf for solids. This is provided exactly due to the problem you describe.

[cgswjs]

Originally Posted by arjun

Starccm has dual under-relaxation and you can set high urf for solids and lower explicit urf for solids. This is provided exactly due to the problem you describe.

I tried your method and the temperature still not updating. I put 0.5 for fluid URF and 1 for solid URF under segregated energy tab. Other URFs were left unchanged. Any idea why?

[arjun]

Originally Posted by cgswjs

I tried your method and the temperature still not updating. I put 0.5 for fluid URF and 1 for solid URF under segregated energy tab. Other URFs were left unchanged. Any idea why?

Could you run few iterations with 0.99 in fluid too. You should know that when you make model unsteady it behaves as if it has under-relaxation due to time step size. So basically the behaviour is similar to steady solver with more under-relaxation).

[cgswjs]

Originally Posted by arjun

Could you run few iterations with 0.99 in fluid too. You should know that when you make model unsteady it behaves as if it has under-relaxation due to time step size. So basically the behaviour is similar to steady solver with more under-relaxation).

I will try it later. I did change time step and max iteration criteria this afternoon and I got a very high residual to 1e50 right after I started the simulation. I think I need to test for the right time step.

[arjun]

Originally Posted by cgswjs

I will try it later. I did change time step and max iteration criteria this afternoon and I got a very high residual to 1e50 right after I started the simulation. I think I need to test for the right time step.

What you need to do is to start with largest values of urf possible and largest timestep that make sense to you. Monitor the plots. It might diverge in few iterations but you can see that temperature profile changes.


Now reduce the timestep , keeping urf intact and you will see that it becomes more and more stable. For flow you have 'Dynamic Local Under-Relaxation' option to optimize the urf. What you need is similar option for Energy too.



This option guess the urf that shall be not too small but enough to run the simulation.

[cgswjs]

Originally Posted by arjun

What you need to do is to start with largest values of urf possible and largest timestep that make sense to you. Monitor the plots. It might diverge in few iterations but you can see that temperature profile changes.


Now reduce the timestep , keeping urf intact and you will see that it becomes more and more stable. For flow you have 'Dynamic Local Under-Relaxation' option to optimize the urf. What you need is similar option for Energy too.



This option guess the urf that shall be not too small but enough to run the simulation.

Thank you. This is what I did this afternoon. I got some temperature on one of the fluid regions. But the residuals start diverging from 5th iteration. I will try the method you said.

[flotus1]

I don't think playing with URFs and global time step sizes will get you very far. Transient CHT needs a different approach.
With version 2019.3 CCM+ got a new feature, that allegedly helps with transient CHT: separate time scales for different regions. You should find it under tools->time scales
Disclaimer: I never used it

[cgswjs]

Originally Posted by flotus1

I don't think playing with URFs and global time step sizes will get you very far. Transient CHT needs a different approach.
With version 2019.3 CCM+ got a new feature, that allegedly helps with transient CHT: separate time scales for different regions. You should find it under tools->time scales
Disclaimer: I never used it

I tried to lower the URF and enabled dynamic local URF. I also readjusted my time step and I got the residuals converging. At least it's not diverging to me. However, the temperature is not changing too much. I've just ran it for 250 iterations and I got a message of 'Stopping criterion ImplicitUnsteadySolver::Minimum Inner Iterations satisfied.' I'm not sure what this means and I lowered my minimum inner iterations to see what happens. Here's some pictures for my residuals and the temperature profile. I expect the temperature of the air in the outer shell to rise but it stays at 27C. Any suggestiongs?

[arjun]

Originally Posted by cgswjs

I tried to lower the URF and enabled dynamic local URF. I also readjusted my time step and I got the residuals converging. At least it's not diverging to me. However, the temperature is not changing too much. I've just ran it for 250 iterations and I got a message of 'Stopping criterion ImplicitUnsteadySolver::Minimum Inner Iterations satisfied.' I'm not sure what this means and I lowered my minimum inner iterations to see what happens. Here's some pictures for my residuals and the temperature profile. I expect the temperature of the air in the outer shell to rise but it stays at 27C. Any suggestiongs?

know that dynamic local urf only work within flow model and has no effect on energy.



If you have access to starccm support then you shall let them know of the problem. Because they can look into the set up and see why it is happening. The behaviour of energy model seem strange at this point to me.

[Ford Prefect]

Originally Posted by flotus1

I don't think playing with URFs and global time step sizes will get you very far. Transient CHT needs a different approach.
With version 2019.3 CCM+ got a new feature, that allegedly helps with transient CHT: separate time scales for different regions. You should find it under tools->time scales
Disclaimer: I never used it

Would the same behavior appear in multiphase flows that also exhibit large differences in conductivity between phases? Does Star-CCM+ use a similar method then, or are you limited to URF modification of the energy equation per phase?