[Muzz]

Originally Posted by me3840

I didn't save the file after I meshed it, I didn't think there was much point.

I wouldn't run a solution up until you get the grid you want. What's your current one look like?

There's my trial mesh... Volume base size 20.0m for fluid domain... 50% base for larger volumetric control and 25.0% base of smaller volumetric controller...

Since I'm meshing the domain using Geometry > Operations, I've lost the ability to apply wake refinement in Regions > Body...

[me3840]

You can do wake refinements using either meshing method. For parts-based meshing, wake refinements are done using a surface control. Create a surface control under custom controls under your mesh operation. There you will find a wake refinement option.

Check out your prism layer thickness, it is probably too high. I would set the thickness to an absolute value rather than a percentage.

[me3840]

Also you have prisms growing on the walls of your domain, which is not desirable.

[Muzz]

Originally Posted by me3840

I didn't save the file after I meshed it, I didn't think there was much point.

I wouldn't run a solution up until you get the grid you want. What's your current one look like?

Instead of using wake refinement, I've added a 3rd volumetric control which spans the two buildings. However, if you look at the attached mesh, I have a bunch of split cells all over the place. How can I get a neater, trimmed mesh?

[me3840]

Do you see on the surface how the lines of the trimmed mesh look bent? This is because the subsurface generator is having trouble aligning the normals to get a quality prism mesh. Your prism layers are probably too thick. If you decrease the size of the prism layer the code will have to do less cell splitting to get a quality mesh. Also ensure that aligned meshing is enabled.

[Muzz]

Originally Posted by me3840

Do you see on the surface how the lines of the trimmed mesh look bent? This is because the subsurface generator is having trouble aligning the normals to get a quality prism mesh. Your prism layers are probably too thick. If you decrease the size of the prism layer the code will have to do less cell splitting to get a quality mesh. Also ensure that aligned meshing is enabled.

Latest version. Prism layers disabled on all surfaces apart from ground and buildings. I'm quite happy with this mesh now...

[me3840]

Now we're talking. You could still do a few more lengths of refinement downstream of the second building. Make sure the wake is refined ~5L downstream, more if you can.

[Muzz]

Originally Posted by me3840

Now we're talking. You could still do a few more lengths of refinement downstream of the second building. Make sure the wake is refined ~5L downstream, more if you can.

Done... Now, worryingly, I ran a laminar simulation using this mesh and it diverged. I know that the base size is still ludicrously big to facilitate mesh optimisation on my terrible desktop but can we talk physics now and refer back to my original problem? For such a simple geometry, I would have thought that a solution would be trivial...

[me3840]

I'm not totally surprised at the laminar result, but it can depend on how it blew up.

What are you using as your initial condition? You should have some kind of velocity set. I'm assuming you're using the segregated solver. There's a lot of air here to get moving, we might need to ramp up the URFs to get it to run okay.

[Muzz]

At the inlet boundary, I've defined the velocity as (x,y,z) table... The table is just a log-law profile with 5m/s at the building height (90m)... For Physics > Initial Conditions, I've just set the velocity as constant with the value being [5.0,0.0,0.0]m/s... Under-relaxation factor for velocity and pressure are both 0.3. The boundaries are: velocity inlet; pressure outlet; wall (ground + buildings); a wall for the ceiling/right hand side boundary and a symmetry condition for the left hand side boundary.

Once I get the laminar simulation solving, I can start modelling the k-omega...

[me3840]

Why not just start with kw right away? Is there data you want to get from the laminar model?

I would not change the default URFs. Rarely if ever will I lower pressure.

Why do you have the ceiling/right as walls? Why not make them symmetry planes or pressure outlets? I doubt there's a giant wall around these buildings.

[Muzz]

I'll do just that then. I kind of wanted to "de-couple" the simulation. I figured if I could get it to converge as a laminar simulation then I knew those input parameters were okay and could focus on turbulence parameters.

As far as the BCs go, I saw it being used as a BC in an external flow problem in one of the tutorials... I had planned to switch back to symmetry conditions for all. I'll do that also... As far as initial conditions go for k-w:

turb intensity = 0.005
turb visc ratio = 0.1
turb length scale = 5m/s

These are the initial physics conditions. However, when defining the inlet boundary conditions, how do these values differ? Are there any rules of thumb for large Re, turbulent, external flow conditions?

Also, is it a good idea to use a transition model? Either Gamma ReTheta or Turbulence Suppression.

[Muzz]

Running k-w with above conditions... Hit with "Turbulent viscosity limited on _ cells in Body 1"... I didn't expect it to run flawlessly with a new mesh but there is clearly still a major problem...

[Muzz]

Had a bit of a breakthrough... Changed steady to implicit unsteady and I'm 500+ iterations in with no turbulent viscosity warnings and good residual values for momentum and continuity... Tke and Sdr aren't converging as well but it's a definite improvement.

[me3840]

I did get a chance to look at your latest mesh you sent via email.

It looks pretty good. I'm not a big fan of how big the cells get just before the outlet, but it may not be a big deal. The only thing I really don't like are:
1. There aren't any prisms on the buildings. kw will probably not enjoy that, but see below.
2. The mesh grows pretty quickly from fine to coarse away from the buildings. Check your y+ values, I'm sure they're extremely high. That can be the source of some of your non-convergence.

As I think I mentioned before, doing a case like this steady isn't easy because the wake is a really transient feature.

For this case I'm unsure if kw is the best choice, ke may be better for a flow like this. Whichever though, I would expect that the dissipation equation be easy to satisfy, but k hard. It's worth making a threshold of the high turbulent viscosity cells to see where the problems are. Furthermore it's also worth it to view the residuals by turning on temporary storage. Where they are high could point to an insufficient mesh sizing.

[Muzz]

Viewed the momentum residuals as a scalar plot. Highest residuals occur in the large cells before the outlet. I decreased the size of those cells. Added prisms to the buildings. Switched to implicit unsteady 2nd order and reduced prism layer size to 0.1m with 20 layers to reduce y+... However, my solution immediately diverged. I had changed the the time-step from 0.001 to 0.01s, so I have now changed it back and started again.

The simulation I ran through the night was absolute garbage. The residuals varied periodically with every 5 iterations, between several orders of magnitude...

EDIT: Change in prism layer thickness has an effect on convergence. Changed back to 2.0m prism layer thickness with 20 layers and the solution is converging again. However, it was converging last night but ended up varying periodically across several orders of magnitude.

EDIT(2):I think I was having problems with using the default number of inner iterations (schoolboy error). Changed those from 5 to 60 and the time step to 0.75s with maximum real time = 75s (The approximate amount of time it takes an individual particle to travel across the inter-building region)

[me3840]

If you're running transient we should expect the residuals to vary several orders of magnitude. In fact if you get several orders of magnitude convergence at each timestep that's super.

Did you start your transient sim from a steady state? that should help out your initial convergence problems.

[Muzz]

Running it steady seems to induce the turbulent viscosity warning. Running it transient from the start reduces the residuals without the viscosity warning. I don't know if this is a solution or just a false indication of one.

I don't think I articulated it well enough. It would vary from E-01 to E-04 for the turbulent residuals. The continuity would vary within E-05 and the momentum residuals would vary in between E-02 to E-06. This seemed like a constant variation with no net decrease in the residuals, if that makes sense. I was kind of expecting a periodic variation around some value once the solution is converged but not one that spans several orders of magnitude. If this is an indication that it is starting to work, why was my vector plot way off?

Running it again with increased inner iterations and increased time-step to make it more appropriate to the scale of the problem.

[Muzz]

Originally Posted by me3840

If you're running transient we should expect the residuals to vary several orders of magnitude. In fact if you get several orders of magnitude convergence at each timestep that's super.

Did you start your transient sim from a steady state? that should help out your initial convergence problems.

Right! I feel like I'm getting close to a solution but curious things are still happening... The attached scalar scene (IsoRough(1)) is from an unsteady 2nd order k-w simulation with 0.75s time-step, 75s physical time and 60 max inner iterations... Residual wise, it didn't seem to converge well and it encountered a turbulent viscosity error.

IsoRough(2) was unsteady second order k-w with 0.75s time-step, 7.5s physical time and 250 max. inner iterations... It converged better and encountered no turbulent viscosity warning...

However, it is plain that, although wrong, IsoRough(1) represents more of a physical solution. IsoRough(2) doesn't even have the representation of the log-law inlet profile present, yet it converged better with no turbulent viscosity error.

Do I need to play around with URFs?

I've attached a diagram of expected result for this type of flow, from the literature. It is the top panel...