# Multilevel Simulations

Navigate: ← Source Terms | Overview

# Multi-level Simulations

In some simulations there are regions of special interest. In these regions strong gradients might occur, so that a higher resolution is required. You then have basically two possibilities to resolve this problem:

1. Increase the global resolution of your simulation. This is generally not a good idea because you very quickly might run into memory problems. A high number of fluid cells also means long computation times.
2. Locally refine the mesh in regions of high interest. You can refine the mesh in regions where it is desired. This focuses the computation cost and memory expenses on the regions where it actually is required. Why waste computation time on flow regions where very little happens? A general problem are the interfaces between grid levels. You can easily get reflections or non-discontinuities there which is why you usually place interfaces in regions where the flow does not fluctuate considerably.

In mus_interpolate_module you can get some background information on the implemented interpolation methods and the general workflow.

## Test Case Description

In this tutorial we cover a channel test case with a cylinder inside. The area around and behind the cylinder is refined by a refinement patch with a higher resolution.

## Mesh Generation

Before starting your simulation you have to set up a mesh again. Again we involve Seeder to generate the required data structures for the solver. It is very advisable to define a variable for the most important variables. Later on you will be able to easily change the resolution of your simulation or some aspect ratio. One very important parameter for setting the resolution of the simulation is a reference tree level that is done in tem_LevelOf.

In our case this will be the tree level of the channel region. Let's name it level and set it based on the computed dx. In our default setting this results in a level of 8. In addition to that, we define the folder (create it via mkdir mesh), the refinement level and the resulting level for the refinement box.

The region around and behind the cylinder is defined by a refinement box. Let's define first, by how many levels we want to refine the elements inside this refined area. For simplicity, let's say that all elements should be on one level higher than the rest of the channel (refinementLevel).

It is also good to have the information about the maximum level in your simulation available as a parameter (maxlevel). You will later on see why.

if useRefine then
refinementLevel  = refinementLevel + 1
-- Refinement level 2 can only be one larger than 1, otherwise level jump is
-- too big.
refinementLevel2 = refinementLevel + 1
end
[...]
maxLevel = level+math.max(refinementLevel, refinementLevel2)
[...]
folder = 'mesh/'


Note: For a description of levels and the layout of the tree have a look at the octree page.

height = 1.0         -- Height of the channel [m]
l_h = 8.0            -- Length to height ratio
length = l_h*height  -- Length of the channel [m]
depth = length       -- Depth of the channel [m]
level =  8           -- General level of mesh refinement


The bounding box, which is the universe in which all elements of the tree will live in, is defined as

bounding_cube = {
origin = { -0.5*length_bnd, -0.5*length_bnd, -0.5*length_bnd+0.5*dx},
length = length_bnd
}


The region around the channel is set to the desired tree level of 9 and 10.

spatial_object = {
[...]
{
attribute = {
kind = 'refinement',
level = refinementLevel+level,
label ='box1'
},
geometry = {
kind = 'canoND',
object = {
origin = { start_x, start_y, start_z },
vec = {
{ size_x, 0.0, 0.0 },
{ 0.0, size_y, 0.0 },
{ 0.0, 0.0, size_z }
}
}
}
},
{
attribute = {
kind = 'refinement',
level = refinementLevel2+level,
label ='box2'
},
geometry = {
kind = 'canoND',
object = {
origin = { start2_x, start2_y, start2_z },
vec = {
{ size2_x, 0.0, 0.0 },
{ 0.0,size2_y, 0.0 },
{ 0.0, 0.0, size2_z }
}
}
}
},
[....]
}
--! [Refinement box 1 & 2]


The rest of the bounding cubic domain is not of interest and hence the discretization level is not of interest.

### Defining Geometry

We need to specify the walls, the inlet, outlet and the cylinder. Let's start with the walls at the north, south position. The walls at east and west direction will later on become the in- and outlet.

[...]
{
attribute = {
kind = 'boundary',
label ='north'
},
geometry = {
kind = 'canoND',
object = {
origin = { -0.5*length-dx_eps, 0.5*height+dx_eps, -0.5*depth-dx_eps },
vec = {
{ length + 2*dx_eps, 0.0, 0.0 },
{ 0.0, 0.0, depth + 2*dx_eps }
}
}
}
},
{
attribute = {
kind = 'boundary',
label ='south'
},
geometry = {
kind = 'canoND',
object = {
origin = { -0.5*length-dx_eps, -0.5*height-dx_eps, -0.5*depth-dx_eps },
vec = {
{ length + 2*dx_eps, 0.0, 0.0 },
{ 0.0, 0.0, depth + 2*dx_eps }
}
}
}
},
[...]
{
attribute = {
kind = 'boundary',
label ='east' -- outlet
},
geometry = {
kind = 'canoND',
object = {
origin = { 0.5*length+dx_eps, -0.5*height-dx_eps, -0.5*depth-dx_eps },
vec = {
{ 0.0, height + 2*dx_eps, 0.0 },
{ 0.0, 0.0, depth + 2*dx_eps }
}
}
}
},
{
attribute = {
kind = 'boundary',
label ='west' -- inlet
},
geometry = {
kind = 'canoND',
object = {
origin = { -0.5*length-dx_eps, -0.5*height-dx_eps, -0.5*depth-dx_eps },
vec = {
{ 0.0, height + 2*dx_eps, 0.0 },
{ 0.0, 0.0, depth + 2*dx_eps }
}
}
}
},


For defining the cylinder or sphere, we use an STL file. This file was before generated by Blender, but you can basically use any software you like for generating such geometry data. The files are located in the test case directory: stl/*.stl. Let's include the sphere STL file with:

   stlfile  = 'stl/sphere.stl'
stlLabel = 'sphere'


then add is to spatiatl_object tabel.

  table.insert(spatial_object,
{
attribute = {
kind = 'boundary',
level = maxLevel,
label = stlLabel,
calc_dist = qValues,
},
geometry = {
kind = 'stl',
object = {
filename = stlfile,
}
},
transformation = {
-- Deformation factor to scale the obstacle. Here: 1 --> remains the same.
deformation =  1,
-- In this case, we do not have to move the geometry.
translation =  { 0.0, 0.0, 0.0 }
}
}
)


One very important action is the placement of the seed. The seed determines the contiguous flow domain. It basically defines for the shapes, what is inside and what is outside. We palce it right in the middle of the channel, which is simply

spatial_object = {
{
attribute = {
kind = 'seed'
},
geometry = {
kind = 'canoND',
object = {
origin = { 0.0, 0.0, dx_half*0.5 },
}
}
},
[...]


Ok. Now we have defined all geometric constraints. Let's continue with refining some parts of the simulation domain.

### Defining Refined Regions

You first need to specify the origin of this box and its extents. Again, we use some variables depending on the total bounding cube.

--! [Refinement box 1]
-- Size of refinement box 1 in x-direction
size_x = 0.75*length
-- Start of refinement box 1 (x)  based on length
start_x = -0.425*length
-- Size of refinement box 1 in y-direction
size_y = 0.5*height
-- Start of refinement box 1 (y)  based on height
start_y = -0.25*height
-- Size of refinement box 1 in y-direction
size_z = 0.5*height
-- Start of refinement box 1 (z)  based on height
start_z = -0.25*height
--! [Refinement box 1]

--! [Refinement box 2]
-- Size of refinement box 2 in x-direction and start of it
start2_x = -0.375*length
size2_x  = 0.5*size_x
-- Size of refinement box 2 in y-direction and start of it
size2_y  = 0.5 * size_y
start2_y = -0.5* size2_y
-- Size of refinement box 2 in z-direction and start of it
size2_z  = size2_y - dx_half
start2_z = start2_y + dx_half/2.0
--! [Refinement box 2]


The patch will then lie around and behind the cylinder.

spatial_object = {
[...]
--! [Refinement box 1 & 2]
{
attribute = {
kind = 'refinement',
level = refinementLevel+level,
label ='box1'
},
geometry = {
kind = 'canoND',
object = {
origin = { start_x, start_y, start_z },
vec = {
{ size_x, 0.0, 0.0 },
{ 0.0, size_y, 0.0 },
{ 0.0, 0.0, size_z }
}
}
}
},
{
attribute = {
kind = 'refinement',
level = refinementLevel2+level,
label ='box2'
},
geometry = {
kind = 'canoND',
object = {
origin = { start2_x, start2_y, start2_z },
vec = {
{ size2_x, 0.0, 0.0 },
{ 0.0,size2_y, 0.0 },
{ 0.0, 0.0, size2_z }
}
}
}
},
--! [Refinement box 1 & 2]
[...]
}


Once you followed through the above explanations, you can visualize the generated mesh. Therefore use Seeder Harvesting.

First, we prepare the config file, defining the folder of the mesh files, the output folder for the vtk file (create the folder first) and the output itself. We name the file sdr_harvester.lua.

mesh          = 'mesh/'
output_folder = 'mesh/'
output = {
format   = 'vtk',
dataform = 'binary',
write_pvd = false
}


Then we can run Seeder Harvesting with: ~/apes/seeder/build/sdr_harvesting harvester.lua

## Setting up the Musubi Configuration

After generating the mesh above, we need to tell Musubi that it should use the above generated mesh. The mesh was stored in the folder mesh. Let's define that along with a name for the simulation

mesh = './mesh/' -- Mesh information
simulation_name = 'channelRefine'


### Initial and Boundary Conditions

Initial conditions are set to a medium with constant pressure and velocity ic_velX.

--! [Initial conditions]
initial_condition = { pressure  = ic_pressure,
velocityX = ic_velX,
velocityY = 0.0,
velocityZ = 0.0,
Sxx = ic_Sxx,
Syy = ic_Syy,
Sxy = ic_Sxy
}
--! [Initial conditions]


Next, we define the variable table for the boundary conditions:

--! [User defined variables]
-- Mainly used for tracking.
-- This variable can be refered to as variable in boundary condition and source
variable = {
-- Reference pressure dependent on physicsModel
{
name='pressureRef',
ncomponents=1,
vartype = 'st_fun',
st_fun = pressureRef
},
-- Pressure at inlet
{
name='pressureIn',
ncomponents=1,
vartype = 'st_fun',
st_fun = pressureIn
},
-- Pressure at outlet
{
name='pressureOut',
ncomponents=1,
vartype = 'st_fun',
st_fun = pressureOut
},
-- Reference shear stress
{
name='stressRef',
ncomponents=1,
vartype = 'st_fun',
st_fun = stressRef },
-- Difference between numerical pressure and reference pressure
{
name='press_diff',
ncomponents=1,
vartype = 'operation',
operation = {
kind = 'difference',
input_varname = { 'pressure_phy', 'pressureRef',},
},
},
}
--! [User defined variables]


The boundary conditions are a little bit more complex, as we have solid walls, the cylinder, and also an inlet and an outlet. Let's start with the wall boundaries. These include among the walls, which we named according to the directions and the cylinder, which we simply called obs. They all get the property of a simple wall.

--! [Boundary conditions]
-- Label is a boundary identifier and it should be same as in seeder
-- configuration.
boundary_condition = {
{  label = 'north',
kind  = 'wall'
},
{  label = 'south',
kind  = 'wall'
},
[...]


For the outlet, we would like to have a pressure_expol "simple pressure" boundary condition, with pressure set to pressureOut a variable we defined in the variable table above.

[...]
{  label = 'east',
kind  = 'pressure_expol',
pressure = 'pressureOut'
}
[...]


For the inlet we also use pressure_expol boundary condition.

[...]
{  label = 'west',
kind  = 'pressure_expol',
pressure = 'pressureIn'
},
[...]


If we set usePeriodic=false we need to define top and bottom as wall. If we use periodic Seeder will handle the periodic relationship for these planes.

-- If we deactivated usePeriodic in seeder.lua, we have to add boundaries for
-- top and bottom.
if usePeriodic ==false then
table.insert( boundary_condition,
{  label = 'top',
kind = 'wall'
}
)
table.insert( boundary_condition,
{
label = 'bottom',
kind = 'wall'
}
end


### Other Simulation Parameters

tmax_phy = 10.0
tmax_iter =  math.ceil(tmax_phy/dt)
interval_phy = tmax_phy/10.0
trac_start = 0.0
rest_start = tmax_phy/4.0
sim_control = {
time_control = {
max = { sim = tmax_phy },
interval = { sim = interval_phy },
clock = 3600 --s
},
[...]
}


### Tracking

We have several different trackers defined. These can be found inside the tracking table. Tracking has been explained in [chapter 03]

tracking = {
-- Track pressure at the center of the channel over time.
{
label = 'probeAtCenter',
--label = 'probePressure',
folder = 'tracking/',
variable = {'pressure_phy'},
shape = {
kind = 'canoND',
object = {
origin = { 0.0, 0.0, 0.0 }
}
},
time_control = { min = {iter=1}, interval = {iter=1} },
output = { format = 'ascii' },
},
[...]


### Visualize the Results

For visualisation of ascii or ascii-spatial format files you can use for example Gnuplot or matplotlib module of python. An example script for postprocessing (plot_track.py) can be found inside the example directory.

Navigate: Overview