3.10. Procedural geometry¶
This tutorial shows how to use procedural shapes to define geometry. This capability was introduced in the 21.1 release.
Simple shapes (cylinder and bends) will be defined and combined to create the geometry. Each shape is controlled by parameters. Filters are applied to the shapes to transform (scale, translate, rotate) the geometry, or flip the normal vector orientation (internal vs external flow). Boolean operations are used to combine the shapes.
The primary focus of this tutorial is to build the geometry. This is done in SMS mode (see SMS meshing workflow tutorial for more details).
3.10.1. Create a new project¶
Create a new project by double-clicking on “Blank” template.
Enter a project name and browse to a location for the new project.
If you have not switched to SMS workflow, you will be prompted to switch. Accept SMS mode.
3.10.2. Create the geometry¶
First, create a cylinder:
Go to the Geometry
pane and click the button to add geometry:
Enter the cylinder’s parameters:
Radius =
0.05
m, Height =0.225
m, Resolution =20
Start angle=
0
deg, end angle =360
deg, resolution =32
Check the
Bottom cap
andTop cap
check boxes and set the resolution to5
for both caps.
Next, create a bend:
Go to the Geometry
pane:
Choose ->
Procedural > Bend
as the geometry input (named “bend”).Enter the bend’s parameters:
Front section: Radius =
0.02
m, Length =0.05
m, Resolution =10
Back section: Radius =
0.05
m, Length =0.25
m, Resolution =20
Bend section: Major radius =
0.075
m, Minor radius =0.02
m, Start angle=0
deg, end angle =90
deg, resolution =16
Circumference: Start angle=
0
deg, end angle =360
deg, resolution =16
Check the
Bottom cap
andTop cap
check boxes and set the resolution to3
for both caps. Leave Offset =0
Rotate and translate the bend:
Combine the cylinder and the bend (union):
Next, create another bend:
Go to the Geometry
pane:
Choose ->
Procedural > Bend
as the geometry input (namedbend1
).Enter the bend’s parameters:
Front section: Radius =
0.02
m, Length =0.1
m, Resolution =10
Back section: Radius =
0.02
m, Length =0.1
m, Resolution =10
Bend section: Major radius =
0.05
m, Minor radius =0.02
m, Start angle=0
deg, end angle =90
deg, resolution =10
Circumference: Start angle=
0
deg, end angle =360
deg, resolution =16
Check the
Bottom cap
andTop cap
check boxes and set the resolution to3
for both caps. Leave Offset =0
Rotate and translate the bend:
3.10.3. Check the geometry orientation¶
Visualize and flip the orientation (normal vectors) of the geometry:
In the model window, show the Geometry, hide the Background mesh, Hide the Regions (visibility is toggled by clicking on each icon). Set the Geometry style to
edges
, opacity to 1.0, check theShow normals
box, set theScale
to 0.01, setcount
to 10,000 (to show all normals).
The normal vectors must point towards the fluid region (here towards the inside of the geometry). However we see that the normals point in the opposite direction (outwards the fluid region). This means we need to flip the normals to correct the orientation.
Select the
union1
geometry,Add a filter: ->
flip normals
. Now the vectors point towards the fluid region. The tips of the arrows are not visible, but we can see the origin (shown as a dot at the center of each face).
Toggle the Region visibility back on.
In
Domain extent
, enter the following:X-direction: Min =
-0.055
m, Max =0.055
m.Y-direction: Min =
0.01
m, Max =0.35
m.Z-direction: Min =
-0.1
m, Max =0.18
m.
Note that the inlets and outlet extend beyond the domain extents. This is intentional, as it usually provides a cleaner intersection and easier way to define boundary conditions regions when they are aligned with the domain box (planes along x=xmin, x=xmax etc.).
3.10.4. Create boundary conditions regions¶
Go to the Regions
pane:
There is already a
Background IC
that is predefined in the Blank template. We can ignore it for now.Click the (top) button to create a new region to be used by a mass inflow boundary condition.
Select
Mass inflow
in the Boundary type drop down menu.Enter a name for the region in the Name field (“top inlet”).
Change the region color to red.
Click the (bottom) button to create a new region to be used by another mass inflow boundary condition.
Select
Mass inflow
in the Boundary type drop down menu.Enter a name for the region in the Name field (“bottom inlet”).
Change the region color to pink.
Click the (back) button to create a new region to be used by pressure outlet boundary condition.
Select
Pressure outflow
in theBoundary type
drop down menu.Enter a name for the region in the Name field (“outlet”).
Change the region color to yellow.
Click the (all) button to create a new region that covers the entire domain to be used for the wall boundary condition.
Select
No-slip wall
in theBoundary type
drop down menu.Enter a name for the region in the
Name
field (“wall”).Change the region color to green.
Check
Select facets (STL)
andflip_normals
, useall
for the selection method. You should see that there are 4003 facets selected.
Note
The pressure outlet and mass inflow boundaries are located along the domain box. They are defined as rectangular 2D regions and must overlap the actual boundary areas (intersection of the STL file with the box planes). The exact boundary area will be computed automatically when preprocessing is performed.
Click the (all) button to create a new region that will be used as initial condition region. This is not needed to generate the mesh, but will be used later when setting up the simulation.
Leave the
Boundary type
asNone
.Enter a name for the region in the
Name
field (“init bed”).Change the region color to black.
Set the Y-extent form
ymin
to0.15
m.
3.10.5. Setup the mesh¶
Go to the Mesh
pane, Background
sub-pane:
Enter
15
for the x cell value.Enter
35
for the y cell value.Enter
30
for the z cell value.
Go to the Mesh
pane, Mesher
sub-pane:
Set the Facet angle tolerance to
0.0
deg. (The geometry unions have created elongated triangles we need to keep).Click
Generate
.Look at the console output to verify the mesh generation completed successfully.
In the Model view, - hide the Geometry, Background mesh and Regions - show the Boundary_Mesh - set
Color by
tobc_id
, - setStyle
toedges
and opacity to1.0
.The Boundary_Mesh should look like a closed surface with colors matching the boundary conditions regions.
After inspection, the mesh is deemed acceptable and we can move to setting up the simulation (Solver mode). Click Accept
. This will unlock the Modeler tab.
3.10.6. Model settings¶
Switch to the Modeler tab (second tab at the bottom left corner of the GUI).
On the
Model
pane, enter a descriptive text in theDescription
field.Select “Discrete Element Model (MFiX-DEM)” in the
Solver
drop-down menu.Keep all other settings at their default values.
3.10.7. Regions settings¶
We already have set all the regions, there is no change required in this pane.
3.10.8. Fluid settings¶
Change Density to
Ideal gas law
.Keep all other settings at their default values.
3.10.9. Solids settings¶
On the Solids
pane, Materials
sub-pane:
Verify the solids model is already set to “Discrete Element Model (MFiX-DEM)”.
Enter the particle diameter of
0.005
m in theDiameter
field.Enter the particle density of
2700
kg/m3 in theDensity
field.Select the
Solids
pane,DEM
sub-pane.Check the
Enable automatic particle generation
checkbox.Keep all other settings at their default values.
3.10.10. Initial conditions settings¶
On the Initial conditions
pane:
3.10.11. Boundary conditions settings¶
On the Boundary conditions
pane:
Select the
top inlet
region. In theSolids 1
tab, enter0.2
for the volume fraction and-0.2
for the Y-axial velocity.Select the
bottom inlet
region. Stay on theFluid
tab, enter4.0
for the Y-axial velocity.The outlet Boundary Conditions is already set to atmospheric pressure. No changes are needed.
The Wall Boundary Conditions is already set to No-slip wall. No changes are needed.
3.10.12. Numerics settings¶
On the Numerics
pane:
On the Residual pane: set the Fluid normalization to
0.0
and the fluid pressure correction scale factor to1.0
On the Preconditioner tab, set the preconditioner to
None
for all equations.
3.10.13. Output settings¶
On the Output
pane:
On the
Basic
sub-pane, check theWrite VTK output files (VTU/VTP)
checkbox.Select the
VTK
sub-pane.Select “Particle Data” from the ‘Output type’ drop-down menu.
Select the “Background IC” region from the list to save all the particle data.
Click
OK
to create the output.Enter a base name for the
*.vtu
files in theFilename base
field (“Particles”).Change the
Write interval
to0.01
seconds.Select the
Diameter
andTranslational Velocity
checkboxes.
3.10.14. Run settings¶
Save the project by clicking the button.
On the Run
pane:
Set
Stop time
to1.0
.Set
Time step
to0.001
.Set
Maximum time step
to0.01
.Keep all other settings at their default values.
3.10.15. Run the simulation¶
3.10.16. View results¶
Results can be viewed, and plotted, while the simulation is running.