Transient analysis differs extremely from steady state analysis

[Anonymous]

Hi Autodesk Community,

I have issues with simulating a transient heat transfer in a hot air channel. My model is quiet similar to the "Tutorial: Transient Heat Transfer in an EGR Valve" http://help.autodesk.com/view/SCDSE/2016/ENU/?guid=GUID-C00E6FD5-A830-4C3B-B721-EA727355886B

First I have simulated the steady state flow distribution. Then I turned flow off and heat transfer on to solve the transient temperature distribution.

The temperature distribution results were very unlikely. The geometry is symmetrical, the steady state flow distribution is symmetrical too but the temperature distribution is asymmertrical. So I tried to solve the temperature distribution in steady state. The results in steady state analysis were plausible (symmetric).

My question is, why do the results from the transient analysis differ from the steady state analysis and why is the temperature distribution asymmetrical, although the geometry and the flow distribution are symmetrical?

I've attached a .cfz support file.

Very thankful for any help.

Best,

JB

[Jon.Wilde]

I suggest two reasons to begin with:

1. You need to figure out how to avoid recirculation at the inlet with a P=0. I would have a flow rate here instead of a pressure and then a P=0 at the outlet. Right now you have no energy balance and a poorly converged solution (the results cannot yet be trusted)
2. Your mesh is too coarse - check out what it looks like half way through the outlet tube, really we need 5-6 elements across this width, try refining it (or a manual mesh as everything is of a similar size)

A transient analysis might be different to steady state to begin with but over time should end the same (as you are then comparing two similar situations). Bear in mind though that the solution might simply be transient in nature, so maybe steady state is not capturing reality...

Hope that helps,

Jon

[Anonymous]

Hi Jon,

thank you for your help.

I've changed the boundary condition at the inlets to a flow rate and assigned a P=0 to the outlet. There is no more recirculation at the inlet. 

Also I've refined the mesh.

The results are still not plausible and asymmetrical.

I'd appreciate it if you could have a look at it again. I attached another .cfz support file.

Thanks

JB

[Jon.Wilde]

OK, so first question - are you sure you have an even flow rate on both sides?

I think the answer is yes - running it here it is fairly close.

Secondly, you need a longer outlet so that the solution can be stable - note the recirculation here due to the change in cross section. I would have it something like 5x longer.

Finally, what time step size are you using for the transient stage?

How long are you running it for? I tested 60s here and it looks pretty symmetrical.

Thanks,

Jon

[Anonymous]

Hi Jon,

I am positive that the flow rate should be even on both sides. 

I have created a longer outlet. The flow looks stable now (see attached screenshot).

I was using a 1s time step size with 1 inner iteration. The simulation is running for 600s.

Basically what I will need in the end is the temperature profile at certain positions every 6 seconds.

Can you recommend a time step size?

I just used the time step size of 60 seconds with the longer outlet and a fine meshing of 2 million elements in total. The flow is almost perfectly even on both sides, but the temperature is higher on one side than on the other. The longer I run the simulation, the bigger the difference gets (see attached screenshot).

Is the small difference in flow (not perfectly symmetrical) creating such a big difference in the temperature distribution?

Thank you for you help so far.

Best,

JB

[Jon.Wilde]

I used a 0.5s time step with 3 inner iterations, 1s might be OK also though.

I would test both incase your time step is the issue.

I got nearly the same flow on both sides but not quite, it was within about 1%.

What actually might be better is to cut the model in half (and use symmetry along the cut plane), use the reduction in model size to increase the mesh count where you have the flow separating and then you should have more accurate results too! 

[Anonymous]

So to make sure we are running the simulation Identical, here are is my configuration:

Mesh count: 3 million. Boundary Layer Enhancement = On

1. Steady state: Flow = On, Heat Transfer = Off, Intelligent Solution Control = On.

                         - Simulation runs until flow is steady

2. Transient: Flow = Off, Heat Transfer = On, Intelligent Solution Control = Off.

                    - Time Step Size=0.5, Inner Iterations=3, Continue From = s250, Time Steps to Run = 100

Results:

1. The Flow is almost the same on both sides (see "Flow XY-Plot"), but it is not smoothly converged (see "Convergence Plot Flow-Only"). Intelligent Solution control was activated. After 250 Iterations the flow didn't reach a steady state and I stopped the Simulation manually.

2. For the Transient simulation I turned off the Flow, turned Heat Transfer on and continued from s250. The temperature distribution is uneven with a difference off 50 degrees celsius from one side to the other (see "Temperature XY-Plot").

Is the flow you get converged smoothly and does the temperature distribution look similar on your simulation?

Next I'll cut the model in half and run the same simulation using symmetry.

Looking forward to your reply.

Best,

JB

[Jon.Wilde]

OK, I have a few ideas 🙂

To comment on your list:

1. If your flow is not totally balanced, I would also not expect the temperature to be. I suggest this is simply down to mesh, the more you mesh it, the more accurate the solution will be (which is why I think symmetry will be useful)
2. I would say this is expected if the flow is unbalanced

A couple of points from me:

• You must set initial temperature conditions to all volumes inbetween the steady state and transient runs
• Your model must be well converged before moving on to the transient section with a very similar flow on each side (again, save yourself time and divide it 🙂 )
  • I do appreciate this seems like avoiding the issue rather than solving it. I am confident that with more and more mesh you would get far closer though, I am merely attempting to save you some time

Hope that helps,

Jon