Macro Sketch Constraint From Spreadsheet/fr

Description
'''Travail en cours. Elle fonctionne pour moi. Dites-moi si quelque chose ne va pas.'''

Macro qui, par un simple clic sur une cellule du tableur, ajoute une contrainte de longueur à une ligne ou entre 2 points en utilisant un alias ou une adresse de cellule du tableur (ex. C2). Les modifications ultérieures de la feuille de calcul mettront à jour la contrainte. La macro peut créer des alias pour vous.

Il suffit de sélectionner 1 ligne, 2 points ou une contrainte, de cliquer sur une cellule du tableur et d'exécuter la macro. Vous pouvez sélectionner des lignes, des points aux extrémités d'une ligne, des points, un cercle, un arc de cercle.



Utilisation
Si nous exécutons la macro alors que nous n'avons pas encore créé de feuille de calcul, elle nous propose d'en créer une et l'ouvre pour que nous puissions commencer à la remplir.



Ce n'est pas obligatoire mais il est préférable d'avoir des alias dans notre feuille de calcul. La macro peut créer des alias à partir de textes dans les cellules.



1) Sélectionnez :
 * une ligne,
 * deux points (extrémité d'une ligne, centre d'un cercle, etc.)
 * ou une contrainte de longueur



2) Cliquez sur une cellule de la feuille de calcul, avec ou sans alias, qui contient une valeur numérique :



3) Lancez la macro.

4) Sélectionnez le type de contrainte souhaité :



Si la cellule a un alias, la propriété de longueur de la contrainte sera quelque chose comme "Spreadsheet.alias". Dans le cas contraire, il s'agira de quelque chose comme "Spreadsheet.D4".



5) Si la contrainte provoque un conflit dans l'esquisse et que la case "conflict detection" est cochée, la macro propose de supprimer la nouvelle contrainte :



Si vous sélectionnez une contrainte existante, vous pouvez modifier la valeur d'une cellule de la feuille de calcul :



Pour être encore plus précis, si, par exemple, une ligne est horizontale plutôt que verticale, à l'ouverture de la boîte de dialogue, le focus sera sur le bouton permettant d'imposer une contrainte horizontale. Si la ligne est verticale et non horizontale, le focus sera sur le bouton permettant d'imposer une contrainte verticale. Dans les deux cas, il vous suffit d'appuyer sur la touche Entrée si vous êtes satisfait de votre choix.



Liens

 * Forum de discussion (français)
 * Liste des macros
 * Comment installer des macros
 * Personnaliser la barre d'outils

Crédits
Merci à openBrain, mario52 et onekk pour leur aide sur le code! Merci à Roy043 et David69 pour les diverses révisions et améliorations du wiki.

Script
Icône de la barre d'outils

Code
ver 00.02.41 23/03/2023 by 2cv001 Macro_Sketch_Constraint_From_Spreadsheet.FCMacro

__author__ = "2cv001" __title__  = "Macro Sketch Constraint From Spreadsheet" __date__   = "2023/03/23"    #YYYY/MM/DD __version__ = __date__ __icon__   = "https://wiki.freecad.org/Images/1/15/Macro_Sketch_Constraint_From_Spreadsheet.svg" __Wiki__   = "https://wiki.freecad.org/Macro_sketchConstraintFromSpreadsheet"
 * 1) !/usr/bin/env python
 * 2) -*- coding: utf-8 -*-
 * 3) Macro Sketch Constraint From Spreadsheet
 * 4) file name : sketchConstraintFromSpreadsheet.FCMacro
 * 5) == Adds a length constraint to a line or between 2 points             ==
 * 6) == using a spreadsheet cell alias or name (ex. C2).                   ==
 * 7) == Future changes to the spreadsheet will update the constraint.      ==
 * 8) == if necessary, the macro help you to create alias                   ==
 * 9) == USE:                                                               ==
 * 10) == 1) Select 1 line, 2 points or a constraint                         ==
 * 11) == 2) Click on a spreadsheet cell                                     ==
 * 12) == 3) Launch the macro                                                ==
 * 13) ==    if the cell has an alias, the length property will be something ==
 * 14) ==    like 'Spreadsheet.alias'.                                       ==
 * 15) ==    if not, just something like 'Spreadsheet.C2'                    ==
 * 16) == You can select lines, points line, points, circle...               ==
 * 17) == You can't select external objetcs  (next version will be able to   ==
 * 1) ==    if not, just something like 'Spreadsheet.C2'                    ==
 * 2) == You can select lines, points line, points, circle...               ==
 * 3) == You can't select external objetcs  (next version will be able to   ==

import FreeCAD, FreeCADGui from PySide import QtGui, QtCore import PySide2 from PySide2.QtGui import QGuiApplication import PySide from PySide2 import QtWidgets import Draft, Part, Sketcher import itertools import configparser import os from importlib import reload importAliasOk = True

separateur = " "     # typically put " " so blanks will be replaced by nouveauCaract nouveauCaract = ''   #Put for example "_" to have the separators replaced by "_". Put "" to have no separator majuscule = True     #set to True if you want  "Diametre du cercle" to be "DiametreDuCercle" changeTexteCellule = False # the text will only be changed if changeCellText is True. # This does not change anything for the allias itself premierCaractereEnMinuscule = True # Force the first character to be in lower case
 * 1) part code for alias
 * 2) parameters for alias creation
 * 1) parameters for alias creation
 * 1) parameters for alias creation

caracEquivalents = [ ['é','e'],['è','e'],['à','a'],['@','a'],['&','e'],['ç','c'], ['²','2'],["'",],['?',],['"',],['(',],[')',],['#',],                 ['$',],['+',],['-',],['*',],['/',],['\\',] ] def remplaceCartatParEquivalent(caractere):    caracResult = caractere       for couple in caracEquivalents:        if (couple[0] == caractere):            caracResult = couple[1]            break    return caracResult
 * 1) list of characters to be replaced by an equivalent. for example an @ will be replaced by 'a'
 * 2) if you add characters, please send me a private message. Il will eventually add it in my code.
 * 1) replaces a character with its equivalent if it exists

def remplaceCararcDansMot(mot): motResult = mot for caract in mot: a = remplaceCartatParEquivalent(caract) motResult = motResult.replace(caract, a)   return motResult
 * 1) replaces all characters of the word with its equivalent if it exists

def traitementChaineSource(chaineSource, separateur, nouveauCaract, majuscule): chaineResult = '' first = True carctDeSeparation = '' for mots in chaineSource.split(separateur): mots = remplaceCararcDansMot(mots) if (not (first)): carctDeSeparation = nouveauCaract if (majuscule): chaineResult = chaineResult + nouveauCaract + mots[:1].upper + mots[1:] # We use "[:1]" instead of "[0]", # for no crash in case of an empty string (which happens if the cell is empty) else: chaineResult = chaineResult + nouveauCaract + mots if premierCaractereEnMinuscule : chaineResult = chaineResult[:1].lower + chaineResult[1:] return chaineResult
 * 1) If separator is ' ' and nouveauCaract is '_', and majuscule is True
 * 2) transforms "Diametre du cylindre" into "Diametre_Du_Cylindre

def setAlias: sels = Gui.Selection.getSelectionEx # If the user wants to trigger the creation of alias # it is sufficient that he does not select any objects in the sketch # but select cells containing strings in the left hand column # of where he want the alias to be created # so test if an object is selected : # result : False if macro can continue. if len(sels) != 0 and len(sels[0].SubElementNames) != 0 : # something selected return False else : ### Ask the user if he is sure if QtGui.QMessageBox.warning(Gui.getMainWindow,       'Warning', 'You did not select any object in an active sketch.' +          '\nDoes it mean you want to create alias automatiquely for cells at the right of selected cells ?',        QtGui.QMessageBox.Ok | QtGui.QMessageBox.Cancel) == QtGui.QMessageBox.Cancel: # if user dont want return False aw = Gui.getMainWindow.centralWidget.activeSubWindow # Store the active window try : mySpreadSheet = Gui.ActiveDocument.ActiveView.getSheet except : QtWidgets.QMessageBox.warning(Gui.getMainWindow, "Warning", "No active spreadsheet with selected cells.") return True # To get list of all selected cells sel_items = aw.widget.findChild(QtGui.QTableView).selectedIndexes

### We define a function that will return the cell identifier from its row (r) and column (c) numbers ### Numbers start at 0 for the first row/column ### Columns are correctly managed with a 2-letter identifier cellName = lambda r,c:'{}{}{}'.format(chr(c//26 + 64) if c//26 > 0 else '', chr(c%26 + 65), r + 1)

# we check that one of the cells is not a numeric. If not, message and exit for item in sel_items: # The selected cells are scanned cell = cellName(item.row, item.column) # We retrieve the cell ID       activeCellContenu = mySpreadSheet.getContents(cell) f = '' try : f = float(activeCellContenu) except : pass if f != '' : QtWidgets.QMessageBox.warning(Gui.getMainWindow,                "Warning", "There is a number in one of the selected cells." +                 " Alias is not possible. \nTry again after correction") return False for item in sel_items: # The selected cells are scanned cell = cellName(item.row, item.column) # The cell identifier is retrieved next_cell = cellName(item.row, item.column + 1) # We get the ID of the cell next to the right activeCellContenu = mySpreadSheet.getContents(cell) # processing the character string contained in the cell activeCellContenu = traitementChaineSource(activeCellContenu, separateur, nouveauCaract, majuscule) if changeTexteCellule:# if the changeCellText parameter is set to True then we replace the text in the cell mySpreadSheet.set(cell, activeCellContenu) alias = activeCellContenu

try: # Bloc try to recover errors mySpreadSheet.setAlias(next_cell, alias) # The alias is assigned to the right-hand neighbouring cell

except ValueError: # If a "ValueError" is triggered (which happens when the alias is not valid) # The user is warned in the report App.Console.PrintWarning("Can't set alias for cell {} : {} isn't valid\n".format(next_cell, alias)) return True


 * 1) End part code for alias
 * 1) End part code for alias

def isExistSpreadSheet : def firstSpreadSheet(doc = App.ActiveDocument): for obj in doc.Objects: if obj.TypeId == 'Spreadsheet::Sheet': return obj return None mySpreadSheet = firstSpreadSheet if not mySpreadSheet : wantNewSpreadSheet = QtWidgets.QMessageBox.question(None, "No spreadsheet detected",       "No spreadsheet in your document. Create one ?",        QtWidgets.QMessageBox.Yes | QtWidgets.QMessageBox.No)
 * 1) if no spreadsheet detected, ask for a creation
 * 2) return :
 * 3) 'exist' if one already exists
 * 4) 'new' if a new is create
 * 5) 'no' if user does not want it
 * 1) 'no' if user does not want it

if wantNewSpreadSheet == QtWidgets.QMessageBox.Yes: mySpreadSheet = App.activeDocument.addObject('Spreadsheet::Sheet', 'Spreadsheet') mySpreadSheet.ViewObject.doubleClicked return 'new' else : return 'no' return 'exist'

class getConstraintType(QtGui.QDialog): def __init__(self, widgetToFocus = None): super(getConstraintType, self).__init__ self.widgetToFocus = widgetToFocus self.initUI
 * 1) Dialog box
 * 2) Ask user which sort of constraint is required
 * 1) Ask user which sort of constraint is required

def initUI(self): self.setWindowIcon(QtGui.QIcon('dialog_icon.png')) gridLayout = QtGui.QGridLayout option1Button = QtGui.QPushButton(QtGui.QIcon(":/icons/constraints/Constraint_HorizontalDistance.svg"), "") option2Button = QtGui.QPushButton(QtGui.QIcon(":/icons/constraints/Constraint_VerticalDistance.svg"), "") option3Button = QtGui.QPushButton(QtGui.QIcon(":/icons/constraints/Constraint_Length.svg"), "") option1Button.setText("Lenght constrainte X") option2Button.setText("Lenght constrainte Y") option3Button.setText("Lenght constrainte") option1Button.setToolTip("Lenght constrainte X") option2Button.setToolTip("Lenght constrainte Y") option3Button.setToolTip("Lenght constrainte") option1Button.clicked.connect(self.onOption1) option2Button.clicked.connect(self.onOption2) option3Button.clicked.connect(self.onOption3)

option4Button = QtGui.QPushButton(QtGui.QIcon(":/icons/application-exit.svg"), "Cancel") option4Button.setToolTip("Option 4 tooltip") option4Button.clicked.connect(self.onOption4)

gridLayout.addWidget(option1Button, 0, 0) gridLayout.addWidget(option2Button, 0, 1) gridLayout.addWidget(option3Button, 1, 0) gridLayout.addWidget(option4Button, 1, 1)

self.setLayout(gridLayout) self.setGeometry(250, 250, 0, 50) self.setWindowTitle("Choose a constraint type") self.setWindowFlags(QtCore.Qt.WindowStaysOnTopHint) self.choiceConstraint = ''

option1Button.setFocusPolicy(QtCore.Qt.NoFocus) option2Button.setFocusPolicy(QtCore.Qt.NoFocus) option3Button.setFocusPolicy(QtCore.Qt.NoFocus) option4Button.setFocusPolicy(QtCore.Qt.NoFocus)

# set focus to specified widget if self.widgetToFocus == 'DistanceX': option1Button.setFocus elif self.widgetToFocus == 'DistanceY': option2Button.setFocus elif self.widgetToFocus == 'Distance': option3Button.setFocus

# Add checkbox self.checkBox = QtGui.QCheckBox("Conflict detection") self.checkBox.setChecked(True) gridLayout.addWidget(self.checkBox, 2, 0, 1, 2) self.checkBox.clicked.connect(self.onOptionCheckBox)

# read ini file to get last checkBoxState config = configparser.ConfigParser # macroDirectory = FreeCAD.ParamGet("User parameter:BaseApp/Preferences/Macro").GetString("MacroPath") + "\\" macroDirectory = FreeCAD.getUserMacroDir(True) try : filePath = os.path.join(macroDirectory, "sketchConstraintFromSpreadsheet.ini") config.read(filePath) # read ini file to know last time state lasChecked = config.getboolean('DEFAULT', 'save_checkbox_state') self.checkBox.setChecked(lasChecked) except : # print('no ini file. Ini file will be create for next launch') pass

# window positioning centerPoint = QGuiApplication.screens[0].geometry.center self.move(centerPoint - self.frameGeometry.center)

def onOption1(self): self.choiceConstraint = 'DistanceX' self.close

def onOption2(self): self.choiceConstraint = 'DistanceY' self.close

def onOption3(self): self.choiceConstraint = 'Distance' self.close

def onOption4(self): self.choiceConstraint = 'Cancel' self.close

def onOptionCheckBox(self): #macroDirectory = FreeCAD.ParamGet("User parameter:BaseApp/Preferences/Macro").GetString("MacroPath") + "\\" macroDirectory = FreeCAD.getUserMacroDir(True) # Save checkbox state to file filePath = os.path.join(macroDirectory, "sketchConstraintFromSpreadsheet.ini") config = configparser.ConfigParser config['DEFAULT'] = {'save_checkbox_state': str(int(self.getCheckBoxState))} with open(filePath, 'w') as configfile: config.write(configfile)

def getCheckBoxState(self): return self.checkBox.isChecked

def activateSketchEditingWindow: def searchForNode(tree, childName, maxLevel = 0): return recursiveSearchForNode(tree, childName, maxLevel, 1)
 * 1) Give the focus to editing sketch window
 * 2) no parameter
 * 3) use : activateSketchEditingWindow
 * 1) use : activateSketchEditingWindow

def recursiveSearchForNode(tree, childName, maxLevel, currentLevel): try: if tree.getByName(childName): return True; elif maxLevel > 0 and currentLevel >= maxLevel: return False; else: for child in tree.getChildren: if recursiveSearchForNode(child, childName, maxLevel, currentLevel + 1): return True except: pass return False

doc = Gui.ActiveDocument if not doc: QtWidgets.QMessageBox.information(Gui.getMainWindow, "Activate window", "No active document") return views = Gui.ActiveDocument.mdiViewsOfType("Gui::View3DInventor") if not views: QtWidgets.QMessageBox.information(Gui.getMainWindow, "Activate window", "No 3D view opened for active document") return editView = None for view in views: if searchForNode(view.getSceneGraph, "Sketch_EditRoot", 3): editView = view break if not editView: QtWidgets.QMessageBox.information(Gui.getMainWindow, "Activate window", "No 3D view has sketch in edit mode for active document") return for win in Gui.getMainWindow.centralWidget.subWindowList: if editView.graphicsView in win.findChildren(QtWidgets.QGraphicsView): Gui.getMainWindow.centralWidget.setActiveSubWindow(win) break

def featuresObjSelected (mySketch, sel, numOrdreObjSelected, indexExtremite) : indexExtremiteLine = 1 indexObjectHavingPoint = -10 typeIdGeometry = None x, y = 0, 0 isInternalObject=True itemName = sel.SubElementNames[numOrdreObjSelected] # ex Edge5 ( line) tabExternalGeomery = [] for item in ActiveSketch.ExternalGeometry : for objName in item [1] : # to get something like # [('Sketch', 'Edge2'), ('Sketch001', 'Edge2'), ('Sketch001', 'Edge1'), ('Sketch', 'Edge1')] tabExternalGeomery.append((item[0].Name, objName)) if itemName == 'RootPoint' : typeInSubElementName = 'RootPoint' indexObjectHavingPoint = -1 typeIdGeometry = mySketch.Geometry[indexObjectHavingPoint].TypeId x, y = 0, 0 else : # for Edge5, typeInSubElementName ->'Edge' and '5' typeInSubElementName, numInNameStr = [''.join(c) for _, c in itertools.groupby(itemName, str.isalpha)] numInName = int(numInNameStr)
 * 1) to get necessary values for the constraint
 * 2) Parameters :
 * 3) sel : selection of objects (a line, 2 points..).
 * 4) numOrdreObjSelected if we want the first objetc selected or the second.
 * 5) indexExtremite if we want the start point (1) or the end point (2), if exist, of the sel
 * 6) return features of a point
 * 7) - typeIdGeometry : Part::GeomLineSegment ....
 * 8) - typeInSubElementName : Edge, vertex ...
 * 9) - indexObjectHavingPoint index of the object having the point (line...)
 * 10) - indexExtremiteLine index of the ends (points) of the line (= start point or end point)
 * 11) - x, y : coordinates of the point
 * 12) - isInternalObject : True if the objetct is on the active sketch
 * 1) - isInternalObject : True if the objetct is on the active sketch

# only one selected object if typeInSubElementName == 'Edge'and len(sel.SubElementNames) == 1: # selection is only one line indexObjectHavingPoint = numInName - 1 indexExtremiteLine = indexExtremite typeIdGeometry = mySketch.Geometry[indexObjectHavingPoint].TypeId # typeIdGeometry : 'Part::GeomCircle' or 'Part::GeomLineSegment' if typeIdGeometry in ['Part::GeomLineSegment'] : if indexExtremite == 1 : x = mySketch.Geometry[indexObjectHavingPoint].StartPoint.x               y = mySketch.Geometry[indexObjectHavingPoint].StartPoint.y            elif indexExtremite == 2 : x = mySketch.Geometry[indexObjectHavingPoint].EndPoint.x               y = mySketch.Geometry[indexObjectHavingPoint].EndPoint.y    if typeInSubElementName == 'ExternalEdge' : isInternalObject = False indexObjectHavingPoint = - numInName - 2 indexExtremiteLine = indexExtremite externalSketchName, externalGeometryName = tabExternalGeomery[numInName - 1] iTypeExternal, iNumStr = [''.join(c) for _, c in itertools.groupby(externalGeometryName, str.isalpha)] iNumExtGeometry = int(iNumStr) typeIdGeometry = App.ActiveDocument.getObject(externalSketchName).Geometry[iNumExtGeometry - 1].TypeId if len(sel.SubElementNames) == 1 : if typeIdGeometry == 'Part::GeomLineSegment' : if  indexExtremite == 1 : x = App.ActiveDocument.getObject(externalSketchName).Geometry[iNumExtGeometry - 1].StartPoint.x                   y = App.ActiveDocument.getObject(externalSketchName).Geometry[iNumExtGeometry - 1].StartPoint.y                elif indexExtremite == 2 : x = App.ActiveDocument.getObject(externalSketchName).Geometry[iNumExtGeometry - 1].EndPoint.x                   y = App.ActiveDocument.getObject(externalSketchName).Geometry[iNumExtGeometry - 1].EndPoint.y

if typeIdGeometry in ['Part::GeomCircle', 'Part::GeomArcOfCircle'] : x = App.ActiveDocument.getObject(externalSketchName).Geometry[iNumExtGeometry - 1].Center.x           y = App.ActiveDocument.getObject(externalSketchName).Geometry[iNumExtGeometry - 1].Center.y            indexExtremiteLine = 3 # 3 for center

# We selected an internal circle but for center (two objects selected) if typeInSubElementName == 'Edge'and len(sel.SubElementNames) == 2 : typeIdGeometry = mySketch.Geometry[numInName - 1].TypeId if typeIdGeometry in ['Part::GeomCircle', 'Part::GeomArcOfCircle'] : indexObjectHavingPoint = numInName - 1 x = mySketch.Geometry[indexObjectHavingPoint].Location.x           y = mySketch.Geometry[indexObjectHavingPoint].Location.y            indexExtremiteLine = 3 # 3 for center

# We selected a vertex if typeInSubElementName == 'Vertex' : # selection is 2 points. sel is a vertex (a point of a line) : indexObjectHavingPoint, indexExtremiteLine = sel.Object.getGeoVertexIndex(numInName - 1) if indexObjectHavingPoint >= 0 : # internal vertex typeIdGeometry = mySketch.Geometry[indexObjectHavingPoint].TypeId if mySketch.Geometry[indexObjectHavingPoint].TypeId == 'Part::GeomLineSegment' : if indexExtremiteLine == 1 : x = mySketch.Geometry[indexObjectHavingPoint].StartPoint.x                   y = mySketch.Geometry[indexObjectHavingPoint].StartPoint.y                if indexExtremiteLine == 2: x = mySketch.Geometry[indexObjectHavingPoint].EndPoint.x                   y = mySketch.Geometry[indexObjectHavingPoint].EndPoint.y            if mySketch.Geometry[indexObjectHavingPoint].TypeId == 'Part::GeomPoint' : x = mySketch.Geometry[indexObjectHavingPoint].X               y = mySketch.Geometry[indexObjectHavingPoint].Y            # we select a vertex Circle (so the center) if mySketch.Geometry[indexObjectHavingPoint].TypeId in ['Part::GeomCircle', 'Part::GeomArcOfCircle'] : x = mySketch.Geometry[indexObjectHavingPoint].Location.x               y = mySketch.Geometry[indexObjectHavingPoint].Location.y        if indexObjectHavingPoint < 0 : # external vertex = vertex of another sketch isInternalObject = False externalSketchName, externalGeometryName = tabExternalGeomery[-indexObjectHavingPoint-3] iType, iNumStr = [''.join(c) for _, c in itertools.groupby(externalGeometryName, str.isalpha)] iNumExtGeometry = int(iNumStr) typeExternal=App.ActiveDocument.getObject(externalSketchName).Geometry[iNumExtGeometry-1].TypeId typeIdGeometry = typeExternal if typeExternal=='Part::GeomLineSegment' : if indexExtremiteLine == 1 : x = App.ActiveDocument.getObject(externalSketchName).Geometry[iNumExtGeometry-1].StartPoint.x                   y = App.ActiveDocument.getObject(externalSketchName).Geometry[iNumExtGeometry-1].StartPoint.y                if indexExtremiteLine == 0 : x = App.ActiveDocument.getObject(externalSketchName).Geometry[iNumExtGeometry-1].EndPoint.x                   y = App.ActiveDocument.getObject(externalSketchName).Geometry[iNumExtGeometry-1].EndPoint.y            if typeExternal == 'Part::GeomCircle' : x = App.ActiveDocument.getObject(externalSketchName).Geometry[iNumExtGeometry-1].Center.x               y = App.ActiveDocument.getObject(externalSketchName).Geometry[iNumExtGeometry-1].Center.y

if typeInSubElementName == 'Constraint' and len(sel.SubElementNames) == 1 : indexConstraint = numInName - 1 indexObjectHavingPoint = indexConstraint typeIdGeometry = 'Constraint' return typeIdGeometry, typeInSubElementName, indexObjectHavingPoint, indexExtremiteLine, x ,y, isInternalObject

def getGuiObjsSelect(type = ''): tabGObjSelect = [] selections = Gui.Selection.getCompleteSelection for sel in (selections): if hasattr(sel, 'Object'):  # depend freecad version if type == '' or sel.Object.TypeId == type : tabGObjSelect.append(sel.Object) else : obj=App.ActiveDocument.getObject(sel.Name) if type == '' or obj.TypeId == type : tabGObjSelect.append(obj) return tabGObjSelect
 * 1) function returning selected objects at GUI level
 * 2)  = Sketch, SpreadSheet ....
 * 3) parameter :
 * 4) '' = no filter
 * 5) 'Spreadsheet::Sheet' for spreadsheets only
 * 6) 'Sketcher::SketchObject' for sketches etc...
 * 7) output: an array of sketch objects, spreadsheets etc.
 * 1) output: an array of sketch objects, spreadsheets etc.

def main: #initialization sheckBoxConstraintConflicState = False indexConstraint = -1 try : FreeCAD.ActiveDocument.Objects except : QtWidgets.QMessageBox.information(None, "Warning", "No document find") return if isExistSpreadSheet in ['no', 'new'] : return # have a look if user wants alias if importAliasOk : if setAlias: return try : mySketch = ActiveSketch except : QtWidgets.QMessageBox.information(None, "Warning", "Select object must be done in edition mode") activateSketchEditingWindow return
 * 1) Main proceddure
 * 1) Main proceddure

# Part SpreadSheet #-   sheets = getGuiObjsSelect('Spreadsheet::Sheet') for sheet in sheets : Gui.Selection.removeSelection(FreeCAD.ActiveDocument.Name, sheet.Name) try : mySpreadSheet = Gui.ActiveDocument.ActiveView.getSheet except : QtWidgets.QMessageBox.information(None, "Warning",               "1- Select a line or 2 points" +                 "\n 2- go to a spreadsheet" +                 "\n 3- select the cell containing the value." +                 "\n 4- stay in the spreadsheet and launch the macro") activateSketchEditingWindow return mySpreadSheetName = mySpreadSheet.Name # select the Spreadsheet To be able to retrieve the selected cell : mySpreadSheet.ViewObject.doubleClicked # retrieve the selected cell ci = lambda :Gui.getMainWindow.centralWidget.activeSubWindow.widget.findChild(QtGui.QTableView).currentIndex cellCode = '{}{}{}'.format(chr(ci.column//28 + 64) if ci.column//26 > 0 else '', chr(ci.column%26 + 65), ci.row + 1) try: cellContents = float(mySpreadSheet.get(cellCode)) except: QtWidgets.QMessageBox.information(None, "Warning",                "Click on a cell with a numeric value before runing the macro") return cellAlias = App.ActiveDocument.getObject(mySpreadSheetName).getAlias(cellCode)

# Part sketch #   sels = Gui.Selection.getSelectionEx

if len(sels) == 0 or len(sels[0].SubElementNames) == 0 : QtWidgets.QMessageBox.information(None, "Warning", "Anathing is select.\n" +              "Select 1 line, 2 points or a constraint in a sketch before selecting a cell in the spreadsheet") activateSketchEditingWindow return elif len(sels[0].SubElementNames) > 2 : QtWidgets.QMessageBox.information(None, "Warning", "Too many objects selected.\n" +              "Select 1 line, 2 points or a constraint in a sketch before selecting a cell in the spreadsheet") activateSketchEditingWindow return else :

# only one obj selected #       if len(sels[0].SubElementNames) == 1 : # only one obj selected #startPoint of the line (typeIdGeometry1, typeInSubElementName1, indexObjectHavingPoint1, indexExtremiteLine1,                x1 ,y1, isInternalObject1)=featuresObjSelected (ActiveSketch, sels[0], 0, 1) if typeInSubElementName1 == 'Constraint' and len(sels[0].SubElementNames) == 1 : indexConstraint=indexObjectHavingPoint1 elif typeIdGeometry1 == 'Part::GeomLineSegment' : (typeIdGeometry2, typeInSubElementName2, indexObjectHavingPoint2, indexExtremiteLine2,                x2 ,y2, isInternalObject2) = featuresObjSelected (ActiveSketch, sels[0], 0, 2) # two obj selected #       if len(sels[0].SubElementNames) == 2: # two obj selected (typeIdGeometry1,typeInSubElementName1, indexObjectHavingPoint1, indexExtremiteLine1,            x1 ,y1, isInternalObject1) = featuresObjSelected (ActiveSketch, sels[0], 0, 1) (typeIdGeometry2,typeInSubElementName2, indexObjectHavingPoint2, indexExtremiteLine2,            x2 ,y2, isInternalObject2) = featuresObjSelected (ActiveSketch, sels[0], 1, 1)

if ((typeInSubElementName1 not in ('Vertex', 'RootPoint', 'ExternalEdge') \ or typeInSubElementName2 not in ('Vertex', 'RootPoint', 'ExternalEdge'))                   and not(typeIdGeometry1 in ('Part::GeomCircle', 'Part::GeomArcOfCircle') \ and typeInSubElementName1 in ['Edge'])) : QtWidgets.QMessageBox.information(None, "Warning", "2 objects are selected but not 2 points .\n" +                "Select 1 line, 2 points or a constraint in a sketch before selecting a cell in the spreadsheet") activateSketchEditingWindow return

#--   # line or points have been selected have a look if we need to swap points # -   if ((len(sels[0].SubElementNames) == 1 and typeIdGeometry1 in['Part::GeomLineSegment'] )           or (len(sels[0].SubElementNames) == 2 and typeIdGeometry1 in['Part::GeomLineSegment', 'Part::GeomCircle', 'Part::GeomArcOfCircle', 'Part::GeomPoint'] )) :

# ask the user what kind of constraint he wants #       # to give focus on the good button # (Button DistanceX if the two points are more horizontal than vertical) if abs(x1 - x2) > abs(y1 - y2) : buttonHavingFocus = 'DistanceX' else : buttonHavingFocus = 'DistanceY' form = getConstraintType(buttonHavingFocus) form.exec_ # is the checkboxSheced ? sheckBoxConstraintConflicState = form.getCheckBoxState if form.choiceConstraint in ('Cancel', '') : activateSketchEditingWindow return myConstraint = form.choiceConstraint # 'DistanceX' or 'DistanceY' or 'Distance'

if (myConstraint == 'DistanceX' and x1 > x2) or (myConstraint == 'DistanceY' and y1 > y2) : indexObjectHavingPoint1, indexObjectHavingPoint2 = indexObjectHavingPoint2, indexObjectHavingPoint1 indexExtremiteLine1, indexExtremiteLine2 = indexExtremiteLine2, indexExtremiteLine1 isInternalObject1, isInternalObject2 = isInternalObject2, isInternalObject1 x1, x2, y1, y2 = x2, x1, y2, y1

# create constraint #=================================   # get value for constraint if cellAlias == None : cellExpression = mySpreadSheetName + '.' + cellCode else : cellExpression = mySpreadSheetName + '.' + cellAlias # create constraint for internal or external circle if (len(sels[0].SubElementNames) == 1 and typeIdGeometry1 in['Part::GeomCircle', 'Part::GeomArcOfCircle'] ) : indexConstraint = mySketch.addConstraint(Sketcher.Constraint('Diameter' , indexObjectHavingPoint1, cellContents))

# create constraint for line or points elif typeIdGeometry1 != 'Constraint' : # no selected constraint, just line or points #create the constraint indexConstraint = mySketch.addConstraint(Sketcher.Constraint(myConstraint , indexObjectHavingPoint1, indexExtremiteLine1, indexObjectHavingPoint2 , indexExtremiteLine2, cellContents)) # if one external line or only one external circle or two external object # was selected : constraint is a reference if len(sels[0].SubElementNames) == 1 and not isInternalObject1 \ or len(sels[0].SubElementNames) == 2 and not isInternalObject1 and not isInternalObject2 : mySketch.setDriving(indexConstraint, False) # External edge constraint is a reference else : # set the constraint'formula' (ex : 'spreadSheet.unAlias') mySketch.setExpression('Constraints[' + str(indexConstraint) + ']', cellExpression) # put Sketch window ahead activateSketchEditingWindow FreeCADGui.Selection.clearSelection # FreeCAD.ActiveDocument.recompute ActiveSketch.touch ActiveSketch.recompute #if Gui.ActiveDocument.getInEdit == Gui.ActiveDocument.Sketch: #Gui.ActiveDocument.Sketch.doubleClicked

# is ther constraintes conflicts ? if sheckBoxConstraintConflicState : #if App.activeDocument.isTouched: # isTouched is not ok in Daily Freecad if 'Invalid' in mySketch.State : a = QtWidgets.QMessageBox.question(None, "",               "Constraints conflic detected. Cancel constraint creation ? ",                QtWidgets.QMessageBox.Yes | QtWidgets.QMessageBox.No, QtWidgets.QMessageBox.No) if a == QtWidgets.QMessageBox.Yes: mySketch.delConstraint(indexConstraint) FreeCAD.ActiveDocument.recompute

activateSketchEditingWindow return

if __name__ == '__main__': main