[biro]

Hello there,

step by step I gather my experience with CFD. After a succesfull meshing with ICEM, I'm working with CFX now.

I've made my first simulations to start slowly. After that I've made a study for mesh independence for my simulation.
For that my first mesh had ~ 6,5 million hexas. After that I refined the mesh. The second simulation had ~12 million cells.
In both cases I worked with y+ ~= 50 and k-epsilon turbulence-model.

The pictures I atached shows the simulation with 6,5 million cells (~2450 Iterations) and then the simulation with 12,5 million cells.
I think, that the mesh refinement didn't take much influence of the results (except the rms of heat transfer).

Now my question:
What can I do for better results ?
My opinion is to use the SST-turbulence-model instead of k-epsilon and/or to change anything on timescale.
Unfortunately I don't know what I have to do with timescale and how to change it. The only thing I know from the Docu of CFX is, that the simulation will be more instable when I enlarge the timestep.

Can anybody give me some tricks or tips how to handle the simuation/mesh on this point.

Thank you for you answer

Greets

[biro]

for completeness the results for the tempeture on my monitor points

[ghorrocks]

Your simulation is probably not converged tight enough. This FAQ gives some tips: http://www.cfd-online.com/Wiki/Ansys...gence_criteria

[biro]

Thank you for your answer.

I took a look on the residuals in Post. I think, thats not the problem. The max residuals are outside the interesting areas.

I will try do change the timestep.
When I get any results i will report

Greets

[biro]

If I set the physical timestep to the "residence Time", like the FAQ said, the simulation will stop by the first iteration with "Overflow error".

Should I try to increase the physical timescale in more, small steps ?

[JuPa]

Decrease the time step if you are having overflow errors.

And check your setup.

[ghorrocks]

The overflow error is an FAQ as well: http://www.cfd-online.com/Wiki/Ansys...do_about_it.3F

[biro]

Thank you for you answers. I haven't seen the the chapter about the "Overflow error".

I decreased the timestep and after some attempts the simulation starts (with timestep = (residence time)/8).
After some iterations i will increase the timestep.


Thank you for your help!

[biro]

My Simulation has finished, but I have different opinions about converging.

The residuals seems to be godd, but when I look at the imbalances, the p-mass imbalance are to high (about over 3%) (see the picture).
Also the pressure at the interesting point has imbalances.
Are these imbalances ok or are they too large ?

How can I decrease the p-mass imbalance ?
I try to choose a larger timestep, like earlier posts.
Another Idea iss to use the SST-turbulence modell.


My boundaries:
Inlet: total Pressure and total Temp at Inlet
Outlet: Opening with Pressure and Temp
k-epsilon turbulence modell

Thank you for you help!

Greets

[ghorrocks]

Back to this FAQ now: http://www.cfd-online.com/Wiki/Ansys...gence_criteria

Once you have the basic simulation working the most effective way of improving convergence is ALWAYS better mesh quality. Even if you think the mesh is pretty good you can make it better and convergence will be better.

[biro]

I think my mesh has a good quality. I will try to get a better mesh quality, but I think it's difficult.

I hoped there is another answer

[biro]

I worked on my mesh and finished it with essential better quality then before.

But in the results I didn't see plenty changes. Especially the Imbalance of mass is very high. At the monitor points the pressure has unwanted imbalances, too.
I calculated with auto timescale and timescale factor = 1.0.

Right now I run the simulation with auto timescale and timescale factor= 10.0. But I don't realy know, whether there are changes at the results.


In my opinion I followed all steps in the FAQ, which was posted earlier, to get better convergence or is there anybody with other ideas ?
Should I run a transient simulation ?

[ghorrocks]

You are getting a periodic signal in your traces which suggests it is modelling a periodic flow feature like vortex shedding. The FAQ says on this issue:

A physical instability, such as vortex shedding - the fix here is to use a larger timescale, a coarser mesh in the vortex shedding region, decrease the blend factor (if using hybrid differencing) or use a lower order turbulence model. The first option is preferred as the latter options can have accuracy implications.

If these do not work it means that your simulation is transient and cannot be run steady state.

[biro]

Ok, I try to use a larger timestep in my actual simulation. This evening I will have results for that.

How can I find the region of vortex shedding ? So that I can edit my mesh to a coarser mesh in this region.

[ghorrocks]

Put the equation residuals in the results file and look for regions of high residuals.

If there is big shedding you can just look at the velocity vectors and find the region of shedding. It is usually behind a bluff trailing edge of a body.

[biro]

yes, I found the region directly. Just putting streamlines for velocity in cfx post.

I will build a coarser mesh in this region.


and again thank you for the extensive help

[biro]

The shedding region take influence of the interesting flow region, so I decide to try a transient simulation.

If I already change from steady state to transient there are information about "time duration", "time steps" and "initial time" needed. I don't know anything about these values. Is there a guide, which I can read, to understand transient simulation ?

[ghorrocks]

The recommended approach is to use adaptive timesteps. Set it to home in on 3-5 coeff loops per iteration, and make the minimum and maximum allowable time step wide enough that it will never reach it. Then the solver will find the correct time step size by itself.

[biro]

Can I set "Time Duration - Total time" to a high value and stop the simulation on my own, like a steady state simulation, when the results are ok (for my opinion) ? Or should I set a "maximal Number of Timesteps" ?

Can I use the last timestep size from steady state simulation to use as initial timestep and should I set "initial time - option" to "automatic" ?

I think, I should not change the default settings of "First Update Time", "Timestep Update Frequency", "Timestep decrease factor" and "Timestep increase factor".
Is this right ?

[ghorrocks]

Unless you know what you are doing leave all the defaults as they are. You need to define values for the 4 blank cells. If you only care about the final result then make the total time big (1e10) so you can run it and stop it manually when you have the final answer, set the min and max to be small and big (1e-10 and 1e10) and the intial time step what ever your initial steady state time step ended up being.