import numpy as np
from solcore.solar_cell_solver import solar_cell_solver
from solcore.spice import solve_circuit
[docs]def solve_pv_module(solar_cell, options, totalcells=25, bias_start=0, bias_end=75, bias_step=0.1, jscSigma=2e-4,
shading=None):
""" Calculate the IV curve of a PV module made of a certain number solar_cells connected in series in a single string. A certain dispersion to the distribution of photocurrents among cells and shadowing losses can be added to ahoeve more realistic results.
:param solar_cell: A solar cell object containing all the junctions
:param options: A state object with all the options needed to solve the solar cell IV
:param totalcells: Total number of cells in a string
:param bias_start: Initial voltage of the IV curve of the module
:param bias_end: Final voltage of the IV curve of the module
:param bias_step: Step for the bias
:param jscSigma: Width of the distribution of short circuit currents around the ideal (eg: 0.02 = 2%). Default is set to 0.02% to aid convergence
:param shading: Array containing the shading loses for each cell. It can be a 2D array (0 = no shading, 1 = full shading)
:return: A tuple with the array of voltages, currents, a list with the Isc of each junction in each cell and the raw output from SPICE.
"""
# We first start by the solar cell as if it were a normal, isolated cell
solar_cell_solver(solar_cell, 'iv', user_options=options)
# We don't care about this IV curve, in principle, but we care about some of the parameters calculated, like jsc,
# j01 or j02 if calculated from detailed balance. We extract those parameters from the cell
totaljuncs = solar_cell.junctions
area = solar_cell.area if hasattr(solar_cell, 'area') else 1
Rs = max(solar_cell.R_series / area, 1e-14)
cell_temp = solar_cell.T - 273
Isc_array = np.zeros(totaljuncs)
I01_array = np.zeros(totaljuncs)
n1_array = np.zeros(totaljuncs)
I02_array = np.zeros(totaljuncs)
n2_array = np.zeros(totaljuncs)
Eg_array = np.zeros(totaljuncs)
rsh_array = np.zeros(totaljuncs)
for i in range(totaljuncs):
try:
Isc_array[i] = solar_cell(i).jsc * area
I01_array[i] = solar_cell(i).j01 * area
n1_array[i] = solar_cell(i).n1 if hasattr(solar_cell(i), 'n1') else 1
I02_array[i] = solar_cell(i).j02 * area
n2_array[i] = solar_cell(i).n2 if hasattr(solar_cell(i), 'n2') else 2
Eg_array[i] = solar_cell(i).Eg
rsh_array[i] = min(solar_cell(i).R_shunt / area, 1e14) if hasattr(solar_cell(i), 'R_shunt') else 1e14
except AttributeError as err:
raise AttributeError('ERROR in PV module: Junction is missing one essential argument. {}'.format(err))
if shading is not None:
shade = shading.flatten()
assert len(shade) == totalcells
else:
shade = np.zeros(totalcells)
# Calculate the probability distribution for the cells
# Since all cells will not generate the same current, some random scatter can be added to the Isc.
# note that the same random value is applied to all sub-cells in a particular junction.
jsc_random_normal = np.random.normal(0.0, jscSigma, size=totalcells)
# Shift the distribution so it is always <=1 so Isc never exceeds the ideal value,
# and also take into account shading
jsc_random_normal = abs(1 - max(jsc_random_normal) * jscSigma + jscSigma * jsc_random_normal) * (1 - shade)
# We choose to keep track of the sub-cell Isc values so that they can be plotted at the end.
all_Isc_values = []
# Now we start to write the spice file
spice_file = """ * SolCore spice Simulation \n.model bypassdiode d \n"""
nodeCounter = 0
junctionCounter = 0
# We loop over all solar cells and all junctions within each solar cell
for n in range(1, totalcells + 1):
# Defines the lower connection for the bypass diode.
lowerBypassConnection = nodeCounter
temp_isc = []
# Loop through junctions writing the spice code for each junction in turn
for j in range(totaljuncs):
junctionCounter += 1
isc = Isc_array[j] * jsc_random_normal[n - 1]
# Write the spice code for the junction to file
spiceout = spice_junction(junctionCounter, nodeCounter, isc, I01_array[j], I02_array[j], n1_array[j],
n2_array[j], Eg_array[j], rsh_array[j])
spice_file = spice_file + spiceout
nodeCounter = nodeCounter + 1
temp_isc.append(isc) # Save the isc value for later plotting
# Entire cell has been built
all_Isc_values.append(temp_isc) # Add isc values to the main list.
# Add the series resistance
spiceout = 'r{0} {1} {2} {3}\n'.format(2 * junctionCounter - 1, nodeCounter+1, nodeCounter, Rs)
nodeCounter = nodeCounter + 1
spice_file = spice_file + spiceout
# Connect bypass diode. Connections are: lowerBypassConnection & nodeCounter
spiceout = 'd{0} {1} {2} bypassdiode\n'.format(2 * junctionCounter + 1, lowerBypassConnection, nodeCounter)
spice_file = spice_file + spiceout
junctionCounter += 1
spice_file = spice_file + ".OPTIONS TNOM=25 TEMP=" + str(cell_temp) + "\n"
spice_file = spice_file + "vbias " + str(nodeCounter) + " 0\n"
spice_file = spice_file + ".dc vbias " + str(bias_start) + " " + str(bias_end) + " " + str(bias_step) + "\n"
spice_file = spice_file + ".plot dc i(vbias)\n"
spice_file = spice_file + ".end \n\n"
# And the definition of the spice file is finished. Now it's time to solve the problem
raw_data = solve_circuit(spice_file)
voltage = []
current = []
raw_data_in_lines = raw_data.split('\n')
for line in raw_data_in_lines:
if len(line) > 2 and line[1] in '0123456789':
splitstring = line.split()
voltage.append(float(splitstring[0]))
current.append(float(splitstring[1]))
return voltage, current, all_Isc_values, raw_data
[docs]def spice_junction(jc, nc, isc, j01, j02, n1, n2, Eg, rsh):
""" Creates the string representation in SPICE of the junciton defined by the input values.
:param jc: junction counter
:param nc: node counter
:param isc: Short circuit current
:param j01: Reverse saturation current corresponding to ideality factor n1
:param j02: Reverse saturation current corresponding to ideality factor n2
:param n1: Ideality factor, typically = 1
:param n2: Ideality factor, typically = 2
:param Eg: Bandgap of the material the junction is made off
:param rsh: Shunt resistance in the junction
:return: A string representation of the junciton in SPICE
"""
isource = 'i{0} {1} {2} dc {3}\n'.format(jc, nc, nc + 1, isc)
d1 = 'd{0} {1} {2} diode{3} OFF\n'.format(2 * jc - 1, nc + 1, nc, 2 * jc - 1)
d1deff = '.model diode{0} d(is={1},n={2},eg={3})\n'.format(2 * jc - 1, j01, n1, Eg)
d2 = 'd{0} {1} {2} diode{3} OFF\n'.format(2 * jc, nc + 1, nc, 2 * jc)
d2deff = '.model diode{0} d(is={1},n={2},eg={3})\n'.format(2 * jc, j02, n2, Eg)
rshunt = 'r{0} {1} {2} {3}\n'.format(2 * jc, nc + 1, nc, rsh)
junction = isource + d1 + d1deff + d2 + d2deff + rshunt
return junction
if __name__ == '__main__':
out = spice_junction(1, 1, 300, 1e-25, 1e-16, 1, 2, 1.4, 0.0001, 1e10)
print(out)
