How to construct an input XML file

Automated Construction

In order to keep usage errors as low as possible, a supporting script xml-builder.shscript in the ARTSS/tools folder (used from the terminal) is provided for setting up XML files. The xml-builder.sh has built-in options for different solvers:

• Pure advection (--advection)
• Pure diffusion (--diffusion) and turbulent diffusion (--diffturb)
• Pure pressure (--pressure)
• Advection and diffusion (--burgers)
• Navier-Stokes equations for velocity (--ns)
  • with turbulence modelling (--nsturb)
  • with energy equation for temperature (--nstemp)
    • with turbulence modelling (--nstempturb)
    • with passive scalar equation for concentration (--nstempcon)
    • with turbulence modelling (--nstempturbcon)

Mandatory to provide are appropriate initial (--initialconditions) and boundary conditions (--boundaryconditions), which are declared in corresponding txt files. If applicable, also all domain obstacles (--domainobstacles) and all surface patches (--domainsurfaces) have to be explicitly declared via txt files, which the script then parses. In order to build various XML files with different simulation times, time and/ or spatial resolutions or iterations, the entry of multiple parameters for --nx, --ny, --nz, --dt, --tend, and --maxiter is possible by the separation of values with commas. To assure that the different setups are saved in different XML files use the printf specifier %d for multiple files (as in --xml testcase_No_%d.xml).

It is worth mentioning that there is no validation of the chosen (or default) parameters (all shown with ./xml-builder.sh -h).

Example of xml-builder.sh Usage

# 1. To get an overview of the options, type
./xml-builder.sh -h

# 2. To build up a Navier-Stokes solver
# with no external forces in domain [0,1]ˆ3
# with set time and spatial resolution, type e.g.,
./xml-builder.sh --ns \
	--forcefct Zero --forcedir xyz \
	--initialconditions ifile.txt \
	--boundaryconditions bfile.txt \
	--xstart 0. --xend 1. \
	--ystart 0. --yend 1. \
	--zstart 0. --zend 1. \
	--tend 10. --dt 0.01 --nu 0.001 \
	--nx 514 --ny 514 --nz 514 \
	--vtkplots 100 --solavail No \
	--xml filename.xml

Example of an XML input file

An example XML file for solving the Navier-Stokes and energy equation with an LES turbulence model is described below. It utilised the Semi-Lagrangian method for advection, the Jacobi method for diffusion with the Constant Smagorinsky-Lilly method, the explicit Euler method for adding buoyancy forces, a V-cycle multigrid method for pressure.

<?xml version="1.0" encoding="UTF-8" ?>
<ARTSS>
  <physical_parameters>
    <t_end> 300. </t_end>       <!-- simulation end time -->
    <dt> 0.01 </dt>             <!-- time stepping -->
    <nu> 2.44139e-05 </nu>      <!-- kinematic viscosity -->
    <beta> 3.28e-3 </beta>      <!-- thermal expansion -->
    <g> -9.81 </g>              <!-- gravitation -->
    <kappa> 3.31e-5 </kappa>    <!-- thermal diffusion -->
    </physical_parameters>

  <solver description = "NSTempTurbSolver" > 
    <advection type = "SemiLagrangian" field = "u,v,w"/>
    <diffusion type = "Jacobi" field = "u,v,w">
      <max_iter> 100 </max_iter>
      <tol_res> 1e-07 </tol_res>
      <w> 1 </w>
    </diffusion>
    <turbulence type = "ConstSmagorinsky">
      <Cs> 0.2 </Cs>
    </turbulence>
    <source type = "ExplicitEuler" force_fct = "Buoyancy" dir = "y">
    </source>
    <pressure type = "VCycleMG" field = "p">
      <n_level> 6 </n_level>
      <n_cycle> 2 </n_cycle>
      <max_cycle> 4 </max_cycle>
      <tol_res> 1e-07 </tol_res>
      <diffusion type = "Jacobi" field = "p">
        <n_relax> 4 </n_relax>
        <max_solve> 100 </max_solve>
        <tol_res> 1e-07 </tol_res>
        <w> 0.6666666667 </w>
      </diffusion>
    </pressure>
    <temperature>
      <advection type = "SemiLagrangian" field = "T"/>
      <diffusion type = "Jacobi" field = "T">
        <max_iter> 100 </max_iter>
        <tol_res> 1e-07 </tol_res>
        <w> 1 </w>
      </diffusion>
      <turbulence include = "Yes">
        <Pr_T> 0.9 </Pr_T>
      </turbulence>
      <source type = "ExplicitEuler" temp_fct = "Zero" dissipation = "No"/>
    </temperature>
    <solution available = "No"/>
  </solver>

  <domain_parameters>
    <X1> -0.3675 </X1>  <!-- physical domain -->
    <X2> 0.3675 </X2>   <!-- defined by opposing corners -->
    <Y1> -0.06 </Y1>
    <Y2> 0.59 </Y2>
    <Z1> -0.2875 </Z1>
    <Z2> 0.2875 </Z2>
    <x1> -0.3675 </x1>  <!-- computational domain -->
    <x2> 0.3675 </x2>   <!-- defined by opposing corners -->
    <y1> -0.06 </y1>
    <y2> 0.59 </y2>
    <z1> -0.2875 </z1>
    <z2> 0.2875 </z2>
    <Nx> 130 </Nx>      <!-- computational grid resolution -->
    <Ny> 130 </Ny>
    <Nz> 130 </Nz>
  </domain_parameters>
	
  <boundaries>
    <boundary field="u,v,w"
            patch="front,back,left,right,top,bottom"
            type="dirichlet"
            value="0.0" />
		<boundary field="p"
            patch="front,back,left,right,top,bottom"
            type="neumann"
            value="0.0" />
		<boundary field="T"
            patch="front,back,left,right,top,bottom"
            type="dirichlet"
            value="304.64" />
		<obstacle ID="0" field="T"
            patch="front,back,left,right,top"
            type="dirichlet"
            value="423.17" />
  </boundaries>
	
	<initial_conditions usr_fct = "LayersT" dir="y">
		<n_layers> 5 </n_layers>
		<border_1> 0.11 </border_1>         <!-- at cell face -->
		<border_2> 0.23 </border_2>
		<border_3> 0.35 </border_3>
		<border_4> 0.47 </border_4>
		<value_1> 303.64 </value_1>         <!-- in Kelvin -->
		<value_2> 304.04 </value_2>
		<value_3> 305.24 </value_3>
		<value_4> 308.84 </value_4>
		<value_5> 310.54 </value_5>
	</initial_conditions>
	
	<visualisation save_vtk="Yes" save_csv="No">
                <vtk_nth_plot> 100 </vtk_nth_plot>        <!-- every 100th time step, resulting in 4 files (0, 100, 200, 300) -->
	</visualisation>
</ARTSS>

Here, the heat source is defined via boundary conditions. In case of a volumetric heat source prescribing the heat release rate, use (not in combination!)

	<source type = "ExplicitEuler" temp_fct = "GaussST" dissipation = "No">
		<HRR> 50.3 </HRR> <!-- total HRR (in kW) -->
		<cp> 1. </cp> <!-- c_p (in kJ/kgK) -->
		<x0> 0. </x0> <!-- center of Gaussian -->
		<y0> 0.02 </y0>
		<z0> 0. </z0>
		<sigma_x> 0.25 </sigma_x> <!-- FWHM -->
		<sigma_y> 0.6 </sigma_y>
		<sigma_z> 0.25 </sigma_z>
		<tau> 5. </tau> <!-- ramp up time -->
	</source>

Error Sources and Restrictions

Be cautious about potential sources of errors:

• When setting attributes in quotes, never include whitespaces
• The number of levels, <n_level> [...] </n_level>, in the multigrid method must be at least l = max(o-1, p-1, q-1) with Nx=2^o +2, Ny=2^p +2, Nz=2^q +2 for o,p,q being natural numbers (including zero)
• Do not use one cell thick obstacles or multiple obstacles occupying all inner cells (especially when restricting to the lowest level in the multigrid method)

---

Back to Wiki home