# -*- coding: utf-8 -*-
# Author: Ruslan Krenzler.
# Date: 16 December 2017
# Create a elbow-fitting.
# Version 0.3

import math
import csv
import os.path

from PySide import QtCore, QtGui
import FreeCAD
import Spreadsheet
import Sketcher
import Part



tu = FreeCAD.Units.parseQuantity


def GetMacroPath():
	param = FreeCAD.ParamGet("User parameter:BaseApp/Preferences/Macro")
	return param.GetString("MacroPath","")

# This is the path to the dimensions table. 
CSV_TABLE_PATH =  GetMacroPath()+"/alpha-deg-elbow.csv"
# It must contain unique values in the column "Name" and also, dimensions listened below.
DIMENSIONS_USED = ["alpha", "POD", "PID", "H", "J", "M"]


# The value RELATIVE_EPSILON is used to slightly change the size of a subtracted part
# to prevent problems with boolean operations.
# This value does not change the appearance of part and can be large.
# If the original value is L then we often use the value L*(1+RELATIVE_EPSILON) instead.
# The relative deviation is then (L*(1+RELATIVE_EPSILON)-L)/L = RELATIVE_EPSILON.
# That is why the constant has "relative" in its name.
RELATIVE_EPSILON = 0.1

class Error(Exception):
    """Base class for exceptions in this module."""
    pass


class UnplausibleDimensions(Error):
    """Exception raised when dimensions are unplausible. For example if
	outer diameter is larger than the iner one.

    Attributes:
        message -- explanation of the error
    """

    def __init__(self, message):
        self.message = message


class Elbow:
	def __init__(self, document):
		self.document = document
		# Init class with test values
		self.alpha = tu("60 deg")
		self.outerD = tu("3 in")
		self.socketD = tu("2 in")
		self.innerD = tu("1 in")
		self.len1 = tu("4 in")
		self.len2 = tu("5 in")

	@staticmethod
	def toSolid(document, part, name):
		"""Convert object to a solid.
			Basically those are commands, which FreeCAD runs when user converts a part to a solid.
		"""
		s = part.Shape.Faces
		s = Part.Solid(Part.Shell(s))
		o = document.addObject("Part::Feature", name)
		o.Label=name
		o.Shape=s
		return o
	@staticmethod
	def NestedObjects(group):
		res = []
		if group.OutList == []:
			res.append(group)
		else:
			# Append children first.
			for o in group.OutList:
				res += Elbow.NestedObjects(o)
			res.append(group)
		return res

	def checkDimensions(self):
		if not ( (self.alpha > tu("0 deg")) and (self.alpha <= tu("180 deg")) ):
			raise UnplausibleDimensions("alpha %s must be within of range (0,180]"%self.alpha)
		if not ( self.innerD > 0):
			raise UnplausibleDimensions("Inner Diameter %s must be positive"%self.innerD)
		if not ( self.socketD >= self.innerD):
			raise UnplausibleDimensions("Sockeet Diameter %s must be greater than or equal to inner Diameter=%s"%(self.socketD, self.innerD))
		if not ( self.outerD > self.socketD):
			raise UnplausibleDimensions("Outer Diameter %s must be greater than socket Diameter =%s"%(self.outerD, self.socketD))
		if not ( self.len1 > 0):
			raise UnplausibleDimensions("Length len1=%s must be positive"%self.len1)
		if not ( self.len2 > 0):
			raise UnplausibleDimensions("Length len2=%s must be positive"%self.len2)
	
	@staticmethod
	def CreateLineSegment(point_1, point_2):
		""" Create a line segment.
		This function creates the line calling different methods, depending on the version of FreeCAD
		"""
		if hasattr(Part, "LineSegment") and callable(getattr(Part, "LineSegment")):
			return Part.LineSegment(point_1, point_2)
		else:
			return Part.Line(point_1, point_2)

	def createElbowCylinder(self, group, r_cyl, r_bent, alpha, len1, len2):
		"""Create a cylinder with a radius r_cyl with a base on X-Y plane
		and bent it by angle alpha along radius r_bent. Add streight cylinders at the ends

		put all new created objects to a group.
		This should simplify the cleaning up of the intermediate parts.
	
		:param r_cyl: radius of the cylinder in Base.Quantity
		:param r_bent: radius of the path in Base.Quantity
		:param alpha: in Base.Quantity
		:param len1: length of the streight part 1
		:param len2: length of the streight part 2
		"""
		base_sketch = self.document.addObject('Sketcher::SketchObject','BaseSketch')
		base_sketch.Placement = App.Placement(App.Vector(0.000000,0.000000,0.000000),App.Rotation(0.000000,0.000000,0.000000,1.000000))

		# When adding a radius, do not forget to convert the units.
		base_sketch.addGeometry(Part.Circle(App.Vector(0.000000,0.000000,0),App.Vector(0,0,1),r_cyl),False)

		# Add sweeping part into X-Z plane.
		path_sketch = self.document.addObject('Sketcher::SketchObject','PathSketch')
		path_sketch.Placement = App.Placement(App.Vector(0.000000,0.000000,0.000000),App.Rotation(-0.707107,0.000000,0.000000,-0.707107))
		# Note the pskecth is rotatet, therefore y and z coordinates are exchanged (? is it still true)
		# Add a line into to the bottom direction (negative Z).
		line1 = self.CreateLineSegment(App.Vector(0.000000,0.000000,0),App.Vector(-0.000000,-len1,0))
		path_sketch.addGeometry(line1, False)

		# Add the arc part.
		start = (tu("pi rad") - alpha).getValueAs("rad")
		stop = tu("pi rad").getValueAs("rad")
		arc = Part.ArcOfCircle(Part.Circle(App.Vector(r_bent,0,0),App.Vector(0,0,1),r_bent),start, stop)
		path_sketch.addGeometry(arc,False)

		# Find coordinates of the right point of the arc.
		x1 = (1-math.cos(alpha.getValueAs("rad")))*r_bent
		z1 = math.sin(alpha.getValueAs("rad"))*r_bent

		x2 = x1 + math.cos((tu("pi/2 rad")-alpha).getValueAs("rad"))*len2
		z2 = z1 + math.sin((tu("pi/2 rad")-alpha).getValueAs("rad"))*len2
		# Draw a streight line for the right pipe.
		line2 = self.CreateLineSegment(App.Vector(x1,z1,0),App.Vector(x2,z2,0))
		line2_geometry = path_sketch.addGeometry(line2,False)
		# Sweep the parts.
		sweep = self.document.addObject('Part::Sweep','Sweep')
		sweep.Sections=[base_sketch, ]
		sweep.Spine=(path_sketch,["Edge1", "Edge2", "Edge3"])
		sweep.Solid=True
		sweep.Frenet=False # Is it necessary?
		# Hide the sketches.
		Gui.getDocument(self.document.Name).getObject(base_sketch.Name).Visibility = False
		Gui.getDocument(self.document.Name).getObject(path_sketch.Name).Visibility = False
		# Add all the objects to the group.
		group.addObject(base_sketch)
		group.addObject(path_sketch,)
		group.addObject(sweep)
		return sweep
		
	def createElbowPart(self, group):
		# Create a ellbow pipe as a difference of two cylinders
		outer_sweep = self.createElbowCylinder(group, self.outerD/2, self.outerD/2, self.alpha, self.len1, self.len2)
		# Make the inner cylinder a littlebit longer, to prevent nummerical errors
		# wenn calculating the difference.
		inner_sweep = self.createElbowCylinder(group, self.innerD/2, self.outerD/2, self.alpha, 
				self.len1*(1+RELATIVE_EPSILON), self.len2*(1+RELATIVE_EPSILON))
		bent_cut = self.document.addObject("Part::Cut","BentCut")
		bent_cut.Base = outer_sweep
		bent_cut.Tool = inner_sweep
		group.addObject(bent_cut)
		return bent_cut
		
	def create(self, convertToSolid):
		self.checkDimensions()
		"""Create elbow."""
		# Create new group to put all the temporal data.
		group = self.document.addObject("App::DocumentObjectGroup", "elbow group")
		# Create the bent part.
		bent_part = self.createElbowPart(group)
		# Remove cyliders from both ends for sockets
		inner_cylinder1 = self.document.addObject("Part::Cylinder","InnerCylinder1")
		inner_cylinder1.Radius = self.socketD/2
		inner_cylinder1.Height = self.len1*(1+RELATIVE_EPSILON)
		inner_cylinder1.Placement.Base = App.Vector(0,0, -inner_cylinder1.Height)

		inner_cylinder2 = self.document.addObject("Part::Cylinder","InnerCylinder2")
		inner_cylinder2.Radius = self.socketD/2
		inner_cylinder2.Height = self.len2*(1+RELATIVE_EPSILON)
		inner_cylinder2.Placement.Base = App.Vector(0,0, -inner_cylinder2.Height)
		x = (1-math.cos(self.alpha.getValueAs("rad"))) *self.outerD/2
		z = math.sin(self.alpha.getValueAs("rad"))*self.outerD/2
		inner_cylinder2.Placement = App.Placement(App.Vector(x,0,z),App.Rotation(App.Vector(0,1,0),self.alpha))
		cut1 = self.document.addObject("Part::Cut","PipeCut1") 
		cut1.Base = bent_part
		cut1.Tool = inner_cylinder1
		elbow = self.document.addObject("Part::Cut","elbow") 
		elbow.Base = cut1
		elbow.Tool = inner_cylinder2
		group.addObject(elbow)
		if convertToSolid:
			# Before making a solid, recompute documents. Otherwise there will be
			#    s = Part.Solid(Part.Shell(s))
			#    <class 'Part.OCCError'>: Shape is null
			# exception.
			self.document.recompute()
			# Now convert all parts to solid, and remove intermediate data.
			solid = self.toSolid(self.document, elbow, "elbow (solid)")
			# Remove previous (intermediate parts).
			parts = Elbow.NestedObjects(group)
			# Document.removeObjects can remove multple objects, when we use
			# parts directly. To prevent exceptions with deleted objects,
			# use the name list instead.
			names_to_remove = []
			for part in parts:
				if part.Name not in names_to_remove:
					names_to_remove.append(part.Name)
			for name in names_to_remove:
				print("Deleting temporary objects %s."%name)
				self.document.removeObject(name)
			return solid
		return group

class ElbowAlpha:
	"""Create a symetrical alpha° elbow"""
	def __init__(self, document):
		self.document = document
		# setup some test values
		self.alpha = tu("45 deg")
		self.H = tu("4 in")
		self.J = tu("2 in")
		self.M = tu("3 in")
		self.socketD = tu("2 in")
		self.innerD = tu("1 in")
	def create(self, convertToSolid = True):
		elbow = Elbow(self.document)
		elbow.alpha = self.alpha
		elbow.outerD = self.M
		elbow.socketD = self.socketD
		elbow.innerD = self.innerD
		elbow.len1 = self.H - self.J
		elbow.len2 =elbow.len1
		return elbow.create(convertToSolid)

class ElbowAlphaFromTable:
	"""Create a part with dimensions from CSV table."""
	def __init__ (self, document, table):
		self.document = document
		self.table = table
	def create(self, partName, convertToSolid = True):
		elbow = ElbowAlpha(self.document)
		row = self.table.findPart(partName)
		if row is None:
			print("Part not found")
			return
		elbow.alpha = tu(row["alpha"])
		elbow.H = tu(row["H"])
		elbow.J = tu(row["J"])
		elbow.M = tu(row["M"])

		elbow.socketD = tu(row["POD"])
		elbow.innerD = tu(row["PID"])
		part = elbow.create(convertToSolid)
		part.Label = partName
		return part



class CsvTable:
	""" Read coupling dimensions from a csv file.
	one part of the column must be unique and contains a unique key.
	It is the column "Name".
	"""
	def __init__(self, mandatoryDims=[]):
		"""
		@param mandatoryDims: list of column names which must be presented in the CSV files apart
		the "Name" column
		"""
		self.headers = []
		self.data = []
		self.hasValidData = False
		self.mandatoryDims=mandatoryDims
	def load(self, filename):
		"""Load data from a CSV file."""
		self.hasValidData = False
		with open(filename, "r") as csvfile:
			csv_reader = csv.reader(csvfile, delimiter=',', quotechar='"')
			self.headers = csv_reader.next()
			# Fill the talble
			self.data = []
			names = []
			ni = self.headers.index("Name")
			for row in csv_reader:
				# Check if the name is unique
				name = row[ni]
				if name in names:
					print('Error: Not unique name "%s" found in %s'%(name, filename))
					exit(1)
				else:
					names.append(name)
				self.data.append(row)
			csvfile.close() # Should I close this file explicitely?
			self.hasValidData = self.hasNecessaryColumns()

	def hasNecessaryColumns(self):
		""" Check if the data contains all calumns required to create a coupling."""
		return all(h in self.headers for h in (self.mandatoryDims + ["Name"]))

	def findPart(self, name):
		"""Return first first raw with the particular part name as a dictionary."""
		# First find out the index of the column "Name".
		ci = self.headers.index("Name")
		# Search for the first appereance of the name in this column.
		for row in self.data:
			if row[ci] == name:
				# Convert row to dicionary.
				return dict(zip(self.headers, row))
		return None

	def getPartName(self, index):
		"""Return part name of a row with the index *index*."""
		ci = self.headers.index("Name")
		return self.data[index][ci]

class PartTableModel(QtCore.QAbstractTableModel): 
	def __init__(self, headers, data, parent=None, *args):
		self.headers = headers
		self.table_data = data
		QtCore.QAbstractTableModel.__init__(self, parent, *args) 
	
	def rowCount(self, parent): 
		return len(self.table_data) 
 
	def columnCount(self, parent):
		return len(self.headers) 
 
	def data(self, index, role):
		if not index.isValid(): 
			return None
		elif role != QtCore.Qt.DisplayRole: 
			return None
		return self.table_data[index.row()][index.column()] 

	def getPartName(self, rowIndex):
		name_index = self.headers.index("Name")
		return self.table_data[rowIndex][name_index]

	def getPartRowIndex(self, partName):
		""" Return row index of the part with name partName.
		:param :partName name of the part
		:return: index of the first row whose part name is equal to partName
				return -1 if no row find.
		"""
		name_index = self.headers.index("Name")
		for row_i in range(name_index, len(self.table_data)):
			if self.table_data[row_i][name_index] == partName:
				return row_i
		return -1
	def headerData(self, col, orientation, role):
		if orientation ==QtCore. Qt.Horizontal and role == QtCore.Qt.DisplayRole:
			return self.headers[col]
		return None

class MainDialog(QtGui.QDialog):
	QSETTINGS_APPLICATION = "OSE piping freecad macros"
	QSETTINGS_NAME = "elbow alpha user input"
	def __init__(self, table):
		super(MainDialog, self).__init__()
		self.table = table
		self.initUi()
	def initUi(self): 
		Dialog = self # Added 
		self.result = -1 
		self.setupUi(self)
		# Fill table with dimensions. 
		self.initTable()

		# Restore previous user input. Ignore exceptions to prevent this part
		# part of the code to prevent GUI from starting, once settings are broken.
		try:
			self.restoreInput()
		except Exception as e:
			print ("Could not restore old user input!")
			print(e)
		self.show()

# The following lines are from QtDesigner .ui-file processed by pyside-uic
# pyside-uic --indent=0 create-elbow-alpha.ui -o tmp.py
# The file paths needs to be adjusted manually. For example
# self.label.setPixmap(QtGui.QPixmap(GetMacroPath()+"alpha-deg-elbow-dimensions.png"))
# access datata in some special FreeCAD directory.
	def setupUi(self, Dialog):
		Dialog.setObjectName("Dialog")
		Dialog.resize(682, 515)
		self.verticalLayout = QtGui.QVBoxLayout(Dialog)
		self.verticalLayout.setObjectName("verticalLayout")
		self.checkBoxCreateSolid = QtGui.QCheckBox(Dialog)
		self.checkBoxCreateSolid.setChecked(True)
		self.checkBoxCreateSolid.setObjectName("checkBoxCreateSolid")
		self.verticalLayout.addWidget(self.checkBoxCreateSolid)
		self.tableViewParts = QtGui.QTableView(Dialog)
		self.tableViewParts.setSelectionMode(QtGui.QAbstractItemView.SingleSelection)
		self.tableViewParts.setSelectionBehavior(QtGui.QAbstractItemView.SelectRows)
		self.tableViewParts.setObjectName("tableViewParts")
		self.verticalLayout.addWidget(self.tableViewParts)
		self.label = QtGui.QLabel(Dialog)
		self.label.setText("")
		self.label.setPixmap(QtGui.QPixmap(GetMacroPath()+"/alpha-deg-elbow-dimensions.png"))
		self.label.setAlignment(QtCore.Qt.AlignCenter)
		self.label.setObjectName("label")
		self.verticalLayout.addWidget(self.label)
		self.buttonBox = QtGui.QDialogButtonBox(Dialog)
		self.buttonBox.setOrientation(QtCore.Qt.Horizontal)
		self.buttonBox.setStandardButtons(QtGui.QDialogButtonBox.Cancel|QtGui.QDialogButtonBox.Ok)
		self.buttonBox.setObjectName("buttonBox")
		self.verticalLayout.addWidget(self.buttonBox)

		self.retranslateUi(Dialog)
		QtCore.QObject.connect(self.buttonBox, QtCore.SIGNAL("accepted()"), Dialog.accept)
		QtCore.QObject.connect(self.buttonBox, QtCore.SIGNAL("rejected()"), Dialog.reject)
		QtCore.QMetaObject.connectSlotsByName(Dialog)

	def retranslateUi(self, Dialog):
		Dialog.setWindowTitle(QtGui.QApplication.translate("Dialog", "Create alpha° elbow", None, QtGui.QApplication.UnicodeUTF8))
		self.checkBoxCreateSolid.setText(QtGui.QApplication.translate("Dialog", "Create Solid", None, QtGui.QApplication.UnicodeUTF8))

	def initTable(self):
		# Read table data from CSV
		self.model = PartTableModel(self.table.headers, self.table.data)
		self.tableViewParts.setModel(self.model)
		
	def getSelectedPartName(self):
		sel = form.tableViewParts.selectionModel()
		if sel.isSelected:
			if len(sel.selectedRows())> 0:
				rowIndex = sel.selectedRows()[0].row()
				return self.model.getPartName(rowIndex)
		return None

	def selectPartByName(self, partName):
		"""Select first row with a part with a name partName."""
		if partName is not None:
			row_i = self.model.getPartRowIndex(partName)
			if row_i >= 0:
				self.tableViewParts.selectRow(row_i)

	def accept(self):
		"""User clicked OK"""
		# Update active document.  If there is none, show a warning message and do nothing.
		document = App.activeDocument()
		if document is not None:
		# Get suitable row from the the table.
			partName = self.getSelectedPartName()
			createSolid = self.checkBoxCreateSolid.isChecked()
			if partName is not None:
				elbow = ElbowAlphaFromTable(document, self.table)
				elbow.create(partName, createSolid)
				document.recompute()
				# Save user input for the next dialog call.
				self.saveInput()
				# Call parent class.
				super(MainDialog, self).accept()
			else:
				msgBox = QtGui.QMessageBox()
				msgBox.setText("Select part")
				msgBox.exec_()
		else:
			text = "I have not found any active document were I can create an elbow.\n"\
				"Use menu File->New to create a new document first, "\
				"then try to create the elbow again."
			msgBox = QtGui.QMessageBox(QtGui.QMessageBox.Warning, "Creating of the elbow failed.", text)
			msgBox.exec_()
	def saveInput(self):
		"""Store user input for the next run."""
		settings = QtCore.QSettings(MainDialog.QSETTINGS_APPLICATION, MainDialog.QSETTINGS_NAME)
		check = self.checkBoxCreateSolid.checkState()
		settings.setValue("checkBoxCreateSolid", int(check))
		settings.setValue("LastSelectedPartName", self.getSelectedPartName())
		settings.sync()
	def restoreInput(self):
		settings = QtCore.QSettings(MainDialog.QSETTINGS_APPLICATION, MainDialog.QSETTINGS_NAME)
		checkState = QtCore.Qt.CheckState(int(settings.value("checkBoxCreateSolid")))
		self.checkBoxCreateSolid.setCheckState(checkState)
		self.selectPartByName(settings.value("LastSelectedPartName"))


def GuiCheckTable():
	# Check if the CSV file exists.
	if os.path.isfile(CSV_TABLE_PATH) == False:
		text = "This macro requires %s  but this file does not exist."%(CSV_TABLE_PATH)
		msgBox = QtGui.QMessageBox(QtGui.QMessageBox.Warning, "Creating of the elbow failed.", text)
		msgBox.exec_()
		exit(1) # Error

	print("Trying to load CSV file with dimensions: %s"%CSV_TABLE_PATH) 
	table = CsvTable(DIMENSIONS_USED)
	table.load(CSV_TABLE_PATH)

	if table.hasValidData == False:
		text = 'Invalid %s.\n'\
			'It must contain columns %s.'%(CSV_TABLE_PATH, ", ".join(DIMENSIONS_USED))
		msgBox = QtGui.QMessageBox(QtGui.QMessageBox.Warning, "Creating of the elbow failed.", text)
		msgBox.exec_()
		exit(1) # Error
	return table

# Test macro.
def TestAlphaTable():
	document = App.activeDocument()
	elbow = ElbowAlphaFromTable(document, table)
	for i in range(0, len(table.data)):
		print("Selecting row %d"%i)
		partName = table.getPartName(i)
		print("Creating part %s"%partName)
		elbow.create(partName, True)
		document.recompute()
		

table = GuiCheckTable()
form = MainDialog(table)