Contents
- Tutorial 1: Setting up a turbine run
This tutorial will demonstrate how to set up a simple AMR-Wind case with a single turbine, one refinement window, and one sampling plane.
| Setting | Value |
|---|---|
| Turbine | NREL 5MW |
| Wind type | Uniform inflow |
| Wind Speed | 10.0 m/s |
At the end of this tutorial, you should be able to create an input file to run, submit, and postprocess the outputs.
First create the directory where case will be setup and run:
$ mkdir tutorial1
$ cd tutorial1Then launch the amrwind_frontend program:
$ /PATH/TO/amrwind_frontend.pyThis should launch amrwind_frontend and look something like this:
In the Simulation tab, we'll first choose the simulation type and basic run length.
In the Simulation type list, choose both ['FreeStream', 'Actuator'].
Under Time control, choose March with ['const dt'], set
Max time to 100 and dt to 0.1:
Scroll down to the end of the tab, and we'll change some more simulation properties. Under Constant values, change
- Constant density =
1.0 - Constant velocity =
[10.0, 0.0, 0.0]
Also choose ['Laminar'] under the Turbulence model options:
To set up the domain and boundary conditions, click on the Domain tab and add the following information.
Under Domain and mesh, put in the following information:
- Domain corner 1:
[-1000, -500, -500] - Domain corner 2:
[1000, 500, 500] - Mesh size:
[128, 64, 64]
Under Periodic Boundary conditions, check both Periodic in Y and Periodic in Z to make both y and z directions periodic. Then click on [show] next to the Boundary conditions on X faces, and add the following information:
- xlo velocity BC:
mass_inflow - xlo density:
1.0 - xlo face velocity (U,V,W):
[10.0, 0.0, 0.0] - xhi velocity BC:
pressure_outflow
The other fields can be left empty or None:
In the ABL tab, set
- Wind vector to
[10.0, 0.0, 0.0]
You can check the wind speed and direction by pressing [Calc WS/WDir], which should calculate the wind speed as 10.0 m/s and wind direction from 270 degrees:
To see the orientation of the wind vector with respect to the computational domain, we can plot the domain as it's currently set up. Under the Plot menu, select Plot domain:
This window gives several options for plotting items in the the AMR-Wind setup. Right now there are no other items available to plot, so just press the [Plot Domain] button to see the domain:
Then press [Close] to exit the plot domain window.
In the Turbines tab, check the box next to Add turbines to simulation.
Then under Add turbines here, click the New button.
In the name field, add turbine0 (this can be arbitrary.) Then
select NREL5MW ADM NOSERVO under Use turbine type and hit Load.
Fill in the turbine base position, yaw, and density
- Base position =
[0, 0, -90] - Nacelle Yaw =
270.0 - Density =
1.0
Then hit the [Save & Update FAST] button at the bottom to make sure all OpenFAST parameters are consistent.
Finally, hit the [Close] button.
To add a refinement region, select the Refinement tab. Then add
set Max refinement level to 1 to add one level of
refinement.
Press [New] to open the Refinement windows dialog box. Add the information in the following fields:
- Name:
box1-- this can be arbitrary - Type:
GeometryRefinement-- for refinement based on a geometry shape.
Then expand the Geometry refinement details section and add the following information:
- Geometry Names:
box1-- this can be arbitrary - Geometry level:
0-- note that the refinement will be applied on level0to produce refined cells at level1. - Geometry type:
box - Box corner:
[-200, -200, -200] - Box axis 1:
[400, 0, 0] - Box axis 2:
[0, 400, 0] - Box axis 3:
[0, 0, 400]
Then press [Save & Close] to complete the refinement specification.
The last element to be added to the simulation case is a sampling
plane to help visualize the solution. Click on the IO tab, and
click on the sampling option to add sampling probes.
Set the Output freq to 100, and choose
['velocity'] as the variable to plot. Then press [New] to
create a new sampling probe input.
In the Sampling probe dialog window, insert the information in the following fields:
- Name:
xyplane-- this can be arbitrary - Type:
PlaneSampler
Then expand the Sample plane specifications section and add the following:
- Plane num points:
101 51 - Plane origin:
-1000 -500 0 - Plane axis1:
2000 0 0 - Plane axis2:
0 1000 0
Once this is complete, press [Save] and [Close]. Now you
should see that xyplane has been added to the list of probes:
Now that the turbine, refinement regions, and sampling planes have been added, we can replot the domain and see how everything is configured. Under the Plot menu, select Plot domain:
This window should now show that the turbines, sample planes, and grid refinements which can be included in the plot.
If box1 and turbine0 are selected, as in below:
and then [Plot Domain] is pressed, the turbine and refinement configuration is shown:
If xplane and turbine0 are selected, you can see how the sampling
probes cover the domain:
Before running this case, we can check that the inputs have been set up correctly. Under the Run menu, select Check inputs.
The output in the terminal will show the results of the check:
-- Checking inputs --
[ PASS] max_level: max_level = 1 >= 0
[ PASS] dt & CFL: DT and CFL OK
[ PASS] Actuator physics: incflo.physics and ICNS.source_terms OK for Actuators
[ PASS] Actuator FST:turbine0 [turbine0_OpenFAST_NREL5MW/nrel5mw_noservo.fst] exists
[ PASS] Actuator FST:turbine0 CompInflow OK
[ PASS] Actuator FST:turbine0 [turbine0_OpenFAST_NREL5MW/./5MW_Baseline/NRELOffshrBsline5MW_Onshore_AeroDyn15.dat] exists
[ PASS] Actuator FST:turbine0 WakeMod=0 OK
[ PASS] Actuator FST:turbine0 AirDens=1.000000, matches incflo.density=1.000000
[ PASS] Sampling probes:xyplane
Results:
9 PASS
0 SKIP
0 FAIL
0 WARN
If anything is set up incorrectly, it may show up as FAIL or WARN
checks in the results.
To write the input file for AMR-Wind, go to the File menu and
select Save input file (or Save input file As). This will
open up the file dialog window, where you can provide the name of the
file to save (tutorial1.inp in this case):
After it saves the file, you should see the input file and the OpenFAST directory:
$ ls -1
turbine0_OpenFAST_NREL5MW
tutorial1.inpThe file tutorial1.inp should look similar to:
Expand input file
# --- Simulation time control parameters --- time.stop_time = 100.0 # Max (simulated) time to evolve [s] time.max_step = -1 time.fixed_dt = 0.1 # Fixed timestep size (in seconds). If negative, then time.cfl is used incflo.physics = FreeStream Actuator # List of physics models to include in simulation. incflo.verbose = 0 io.check_file = chk incflo.use_godunov = true incflo.godunov_type = ppm turbulence.model = Laminar incflo.gravity = 0.0 0.0 -9.81 # Gravitational acceleration vector (x,y,z) [m/s^2] incflo.density = 1.0 # Fluid density [kg/m^3] transport.viscosity = 1.872e-05 # Fluid dynamic viscosity [kg/m-s] transport.laminar_prandtl = 0.7 # Laminar prandtl number transport.turbulent_prandtl = 0.3333 # Turbulent prandtl number ConstValue.density.value = 1.0 ConstValue.velocity.value = 10.0 0.0 0.0 # --- Geometry and Mesh --- geometry.prob_lo = -1000.0 -500.0 -500.0 geometry.prob_hi = 1000.0 500.0 500.0 amr.n_cell = 128 64 64 # Number of cells in x, y, and z directions amr.max_level = 1 geometry.is_periodic = 0 1 1 xlo.type = mass_inflow xlo.density = 1.0 xlo.velocity = 10.0 0.0 0.0 xhi.type = pressure_outflow # --- ABL parameters --- ICNS.source_terms = ActuatorForcing incflo.velocity = 10.0 0.0 0.0 ABLForcing.abl_forcing_height = 0.0 time.plot_interval = 1000 io.plot_file = plt io.KE_int = -1 incflo.post_processing = sampling # --- Sampling parameters --- sampling.output_frequency = 100 sampling.fields = velocity #---- sample defs ---- sampling.labels = xyplane sampling.xyplane.type = PlaneSampler sampling.xyplane.num_points = 101 51 sampling.xyplane.origin = -1000.0 -500.0 0.0 sampling.xyplane.axis1 = 2000.0 0.0 0.0 sampling.xyplane.axis2 = 0.0 1000.0 0.0 sampling.xyplane.normal = 0.0 0.0 0.0 #---- tagging defs ---- tagging.labels = box1 tagging.box1.type = GeometryRefinement tagging.box1.shapes = box1 tagging.box1.level = 0 tagging.box1.box1.type = box tagging.box1.box1.origin = -200.0 -200.0 -200.0 tagging.box1.box1.xaxis = 400.0 0.0 0.0 tagging.box1.box1.yaxis = 0.0 400.0 0.0 tagging.box1.box1.zaxis = 0.0 0.0 400.0 #---- actuator defs ---- Actuator.labels = turbine0 Actuator.turbine0.type = TurbineFastDisk Actuator.turbine0.openfast_input_file = turbine0_OpenFAST_NREL5MW/nrel5mw_noservo.fst Actuator.turbine0.base_position = 0.0 0.0 -90.0 Actuator.turbine0.rotor_diameter = 126.0 Actuator.turbine0.hub_height = 90.0 Actuator.turbine0.num_points_blade = 64 Actuator.turbine0.num_points_tower = 12 Actuator.turbine0.epsilon = 10.0 10.0 10.0 Actuator.turbine0.epsilon_tower = 5.0 5.0 5.0 Actuator.turbine0.openfast_start_time = 0.0 Actuator.turbine0.openfast_stop_time = 1000.0 Actuator.turbine0.nacelle_drag_coeff = 0.0 Actuator.turbine0.nacelle_area = 0.0 Actuator.turbine0.yaw = 270.0 Actuator.turbine0.output_frequency = 10 Actuator.turbine0.density = 1.0 #---- extra params ---- #== END AMR-WIND INPUT ==
To run the case, there are two possibilities. The case can be run on the local machine, or a submission file can be generated to run on an HPC cluster.
Note that the following instructions require that
amrwind_frontend.py is set up correctly with the right paths and
locations to the executable.
This option can be used if there are sufficient resources on the local machine.
Under the Run menu, select Local run. If properly configured,
most of the executable and paths should not need to be changed.
Provide a Log filename (like log.txt) and set the number of
processors in N processors (default 1).
Then press [Save & Run] to start the run
You can create a submission script for running on the HPC machines. Under the Run menu, select Job submission.
Fill in the following fields:
- submit script filename:
submit.sh - amr_wind executable:
amr_wind(Provide full path if necessary) - job name:
amrwind1(can be arbitrary) - Number of nodes:
4 - Run time:
1:00:00
To see what the submission script looks like, click on [Preview script] button. Then click on [Save script] to write the file.
To submit the job through the interface, hit Submit job, although it can also be done on the command line, e.g., through
$ bsub < submit.shor through SLURM systems:
$ sbatch submit.shUnder the Plot menu, select Fast outputs.
Click on [Add file] and select the file
turbine0_OpenFAST_NREL5MW/nrel5mw_noservo.out. Then click on
[Load/Reload Data] to load the data.
Once the data is loaded, select one of the variables such as Wind1VelX:
Then press [Plot] to plot the FAST output:
In the Postpro tab, scroll down to the Plot Sample Planes tab.
Then press [Choose file] and choose the file
post_processing/sampling00000.nc, and press [Load file]. This
will load the NetCDF data file and show the available groups to plot.
Select xyplane and press [Load variables]
This should load the available variables to plot. Select velocityx
in the NetCDF vars list, and choose X and Y as Plot axis 1
and Plot axis 2, respectively. (AUTO is the automatic option.)
Under Set current time, put 10 (the last data sample).
Then press [Plot Sample] to plot a contour of the x-velocity at the hub-height plane:
