[Jiricbeng]

Hello,

I am simulating transient conjugate heat transfer of a vehicle flying from subsonic to hypersonic regime (from Mach number 0.3 to 5).
The model consists of pressure-far-field boundary condition and walls of the vehicle. The solid of the vehicle is connected by coupled interface (node to node connection, fluid and solid were meshed as one part). The boundary condition are set by transient profile on pressure-far-field, so Pressure, Temperature and Mach number are changing in time.

The vehicle has rotational symmetry and the flow is also symmetric - zero angle of attack. Therefore I created 2D axisymmetric model but I created also 3D 180deg segment model (because another subsequent analysis will include non-zero angle of attack). I want to correlate 2D axisym. model with 3D model. The mesh of 3D model is made by sweep and the sizing is the same as in 2D axisym. model. In both cases it is full hexa mesh.

Converging 2D axisym. model is not any issue, but I cannot reasonably converge 3D model. I did sensitivity study for time-step sizes and for example time-step 0.1s still works fine for 2D axisym. but it does not work for 3D, the results of heat flux are significantly different. It is obvious from contour plots that the flow field is not converged.

Any ideas/comments/recommendation to this issue are appreciated !

[AlexanderZ]

try to use full 3D model

best regards

[Jiricbeng]

Do you have some experience with better convergence for 360deg than 180deg?

[AlexanderZ]

1.looks like you trust in results from 2D case, however, 0.1 sec time step for this kind of simulation is huge from my point of view. By the way, how big your domain is?

2.looks like you think, that mesh quality for 3D case is good enough. BC and settings you take from 2D. So what else can be done?

Full 3D may lead to better convergence.
No information regarding turbulent model.
You may decrease relaxation factors.
You may decrease time step size and increase number of iterations per timestep.

best regards

[Jiricbeng]

1. It is true that I quite believe the 2D case, because all results were the same for different time steps. The domain is about 150 metres large and size of the vehicle is about 1 metre, so more than 70 metres from vehicle is fluid. I calculate double precision because it is CHT and because there are big differences between cell sizes (boundary layer vs far field elements). Moreover double precision significantly improved convergence of the continuity residual.

2. Yeah I assume the mesh quality is acceptable based on y+.

I use K-Omega SST turbulence model.
I tried to increase number of iterations/time step but it does not help very much. But I also tried to reduce time step significantly - up to 0.0002s and it converged well of course. But it is not feasable to calculate in real time. The flight lasts more than 100 seconds.

I also agree that 0.1s is huge, yes it is, and I was a bit surprised how well 2D case converged even for this huge time step.

[AlexanderZ]

from my point of view, you may try to apply adaptive time step size.
start with big value
than decrease significantly on velocity M0.9-M1.1
once the flow is stable, you may increase time step
but, ofc, you should decrease it again of high velocity

You may use DEFINE_DELTAT marcos to make UDF for adaptive time step

best regards

[Jiricbeng]

Just let you know about the progress:

I ran 2D axiym. case with the following timestep and iterations:

timestep size: 5s (yes it is huge)
number of iterations per timestep: 1500

The positive and little bit surprising thing is that I obtained the very same results as in case of timestep 0.005s and 40 iterations per timestep.

Therefore I am running the 3D model with 5s timestep and big number of iterations. Actually, I am searching for temperature development in time and this big time step ensures calculating an average values during 5s timestep, it is like "quasi-steady states obtained by transient analysis".