[AtoHM]

Hi guys, I am facing a problem here which I am unable to resolve.
I got a transient simulation with only water with constant material properties. So no energy equation and incompressible. It is a rectangular tank which is either filled or drained during the simulation according to a hydrograph I have. The period of time I want to simulate is too long to make it two-phase, so I used rigid lid and account for the changing water volume by shifting the "TOP" boundary (water level) with moving mesh.
Unfortunately the solver crashed right in the first time step with overflow. I tried a view things but then got it running in double-precision. Obviously that takes a significant amount of time longer, no way I can use it for the whole simulation, but might be ok for the startup. As I had these startup problems, I created a trn file right after 2 iterations, which I was able to check now. There are pressures of 10^22 Pa inside my domain and the fluid velocity is nowhere near realistic, 10^7 m/s and such. I really have no idea where that originates from. I tried several options of initializing the pressure, ref pressure in domain and material of 0 [atm] or 1 [atm]. As there is no pressure boundary, I explicitly provided a pressure reference location under Solver Control correlating to the two values above (which seems to be ignored by the solver, at least it states another location in the .out file).

Even more odd, the flow rate is very low at the beginning, so I expect nothing to really happen. I also checked the FAQ on overflow again but I considered all that.
I did a similar simulation last year which worked. I used it as template, only changed the flow rate and used another mesh with better quality measures than the old one. After I could'nt sort it out, I decided to run the old simulation again just to see if it still works with the new cfx version. It did, kind of, but during the first 10 iterations there were also these crazy high values.
Knowing that, I gave my new simulation a bit more time to see if the values come down. They do, but waaaay slower than in the old simulation. They are still too high about 100 iterations into the simulation. I could live with it, but I really want to understand where these huge values come from. Why does cfx ignore my pressure and velocity initialization? There is probably something simply wrong in my setup, but it is so simple, I can't see what it could be. Any idea is much appreciated.
Thanks alot and have a nice sunday.

[ghorrocks]

CFX is not ignoring your initial conditions. CFX thinks that your conditions lead to those crazy values. So there is something in your setup or numerics which is causing it.

Please post an image of what you are modelling and the output file.

[AtoHM]

I'm afraid I can't share these publicly. Thanks for your help anyway.
A colleague had some hints which might help - I will try on my own for now and keep this post updated if I can sort it out.
There is at least one issue with my mesh motion expression.

[AtoHM]

I figured it out. It could only be the pressure initialization.
During my failed tests, I used different reference pressure levels cause I thought round off errors might be the problem. The inflow is very small at the beginning and so are the pressure differences. I read through the cfx guides again yesterday regarding these settings. What I didn't think of was the hydrostatic pressure profile I use for initialization - this was however recommended in the manuals, but only for multiphase simulations. I still followed the advice of using the average of max / min expected pressure in the domain as reference pressure and then instead of using the hydrostatic pressure initialization, I used relative pressure = 0 Pa everywhere. And now it runs perfectly. It makes sense, there is no hydrostatic pressure profile w/o gravity.
Anyway, I also found a cfx bug. Since I had a strange mesh displacement issue a few years back, I use an expert parameter called mesh displacement diffusion scheme = 3. When using this parameter, the option mesh motion relative to previous mesh does just not work. It shifts the mesh in the first iteration but never again afterwards. I could confirm this by using the same setup without the expert parameter, it worked perfectly. I will report this to CFX Support.