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.

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
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 00.02.3 02/03/2023 by 2cv001 Macro_Sketch_Constraint_From_Spreadsheet.FCMacro

__author__ = "2cv001" __title__  = "Macro Sketch Constraint From Spreadsheet" __date__   = "2023/03/02"    #YYYY/MM/DD __version__ = __date__ __icon__   = "https://wiki.freecad.org/File:Macro_Sketch_Constraint_From_Spreadsheet.svg" __Wiki__   = "https://wiki.freecad.org/Macro_Sketch_Constraint_From_Spreadsheet"
 * 1) !/usr/bin/env python
 * 2) -*- coding: utf-8 -*-
 * 3) Macro Sketch Constraint From Spreadsheet
 * 4) == Adds a length constraint to a line or between 2 points              ==
 * 5) == using a spreadsheet cell alias or address (ex. C2).                 ==
 * 6) == Future changes to the spreadsheet will update the constraint.       ==
 * 7) == USE:                                                                ==
 * 8) == 1) Select 1 line, 2 points or a constraint                          ==
 * 9) == 2) Click on a spreadsheet cell                                      ==
 * 10) == 3) Launch the macro                                                 ==
 * 11) ==    if the cell has an alias, the length property will be something  ==
 * 12) ==    like 'Spreadsheet.alias'.                                        ==
 * 13) ==    if not, just something like 'Spreadsheet.C2'                     ==
 * 14) == You can select lines, points line, points, circle...                ==
 * 1) ==    like 'Spreadsheet.alias'.                                        ==
 * 2) ==    if not, just something like 'Spreadsheet.C2'                     ==
 * 3) == You can select lines, points line, points, circle...                ==

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

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 #macroDirectory=FreeCAD.ParamGet("User parameter:BaseApp/Preferences/Macro").GetString("MacroPath")+"\\" # LINUX ? 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") + "\\" try : config.read(macroDirectory + 'constraintFromTabIcone.ini') # 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')

# 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") + "\\"

# Save checkbox state to file filePath = os.path.join(macroDirectory, "constraintFromTabIcone.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 itemName=sel.SubElementNames[numOrdreObjSelected] # ex Edge5 ( line) if itemName=='RootPoint' : typeInSubElementName='RootPoint' indexObjectHavingPoint=-1 typeIdGeometry=mySketch.Geometry[indexObjectHavingPoint].TypeId x,y=0,0 else : typeInSubElementName, numInNameStr = [''.join(c) for _, c in itertools.groupby(itemName, str.isalpha)] # Edge5 renvoie'Edge' et '5' numInName=int(numInNameStr) # index de ce qui a été sélectionné =numInName1-1 car commence à 0
 * 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) - typeInSubElementName
 * 8) - indexObjectHavingPoint index of the object having the point (line...)
 * 9) - indexExtremiteLine index of the ends (points) of the line (=start point or end point)
 * -x,y : coordinates of the point
 * -x,y : coordinates of the point

# 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'ou '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        # We selected a circle but for center (two obs selected) if typeInSubElementName == 'Edge'and len(sel.SubElementNames)==2: indexObjectHavingPoint=numInName-1 typeIdGeometry=mySketch.Geometry[indexObjectHavingPoint].TypeId if typeIdGeometry in ['Part::GeomCircle'] : 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) 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 typeInSubElementName=='Constraint' and len(sel.SubElementNames)==1 : indexConstraint=numInName-1 indexObjectHavingPoint=indexConstraint typeIdGeometry='Constraint'

return typeIdGeometry,typeInSubElementName, indexObjectHavingPoint, indexExtremiteLine, x ,y

def procEnd: activateSketchEditingWindow
 * 1) call at end
 * 1) call at end

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 : mySketch=ActiveSketch except : QtWidgets.QMessageBox.information(None,"Warning","Select object must be done in edition mode") return mySketchName=mySketch.Name #actually not use # 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") 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 returning to the sketch") return cellAlias= App.ActiveDocument.getObject(mySpreadSheetName).getAlias(cellCode) # Part sketch #   sels = Gui.Selection.getSelectionEx if 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") 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") return
 * 1) Main proceddure
 * 1) Main proceddure

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)=featuresObjSelected (ActiveSketch, sels[0],0,1) print('(typeIdGeometry1,typeInSubElementName1', typeIdGeometry1,typeInSubElementName1)           if typeInSubElementName1=='Constraint' and len(sels[0].SubElementNames)==1 :                indexConstraint=indexObjectHavingPoint1            elif typeIdGeometry1=='Part::GeomLineSegment' :                (typeIdGeometry2, typeInSubElementName2, indexObjectHavingPoint2, indexExtremiteLine2, x2 ,y2)=featuresObjSelected (ActiveSketch, sels[0],0,2)        # two obj selected            #         if len(sels[0].SubElementNames)== 2: # two obj selected            (typeIdGeometry1,typeInSubElementName1, indexObjectHavingPoint1, indexExtremiteLine1, x1 ,y1)=featuresObjSelected (ActiveSketch, sels[0],0,1)            print('(typeIdGeometry1,typeInSubElementName1, indexObjectHavingPoint1, indexExtremiteLine1, x1 ,y1)',(typeIdGeometry1,typeInSubElementName1, indexObjectHavingPoint1, indexExtremiteLine1, x1 ,y1)) (typeIdGeometry2,typeInSubElementName2, indexObjectHavingPoint2, indexExtremiteLine2, x2 ,y2)=featuresObjSelected (ActiveSketch, sels[0],1,1) print(' 368 typeInSubElementName1',typeInSubElementName1) print(' 368 typeIdGeometry1',typeIdGeometry1) if ((typeInSubElementName1 not in ('Vertex', 'RootPoint') or typeInSubElementName2 not in ('Vertex','RootPoint'))                   and not(typeIdGeometry1 == 'Part::GeomCircle' 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") return # to do : if one is a circle, reolace with it's center. #if typeIdGeometry1 in ('Part::GeomCircle', 'Part::GeomArcOfCircle')

#--   # 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','') : 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

# create constraint #=================================   if cellAlias==None : cellExpression= mySpreadSheetName+'.'+cellCode else : cellExpression= mySpreadSheetName+'.'+cellAlias if (len(sels[0].SubElementNames)== 1 and typeIdGeometry1 in['Part::GeomCircle','Part::GeomArcOfCircle'] ) : print('398 indexObjectHavingPoint1',indexObjectHavingPoint1) indexConstraint=mySketch.addConstraint(Sketcher.Constraint('Diameter', indexObjectHavingPoint1, cellContents)) elif typeIdGeometry1!='Constraint' : # no selected constraint, just line or points #create the constraint indexConstraint=mySketch.addConstraint(Sketcher.Constraint(myConstraint , indexObjectHavingPoint1,indexExtremiteLine1,indexObjectHavingPoint2,indexExtremiteLine2, cellContents)) # for all type, 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 ? ",                QtWidgets.QMessageBox.Yes | QtWidgets.QMessageBox.No, QtWidgets.QMessageBox.No) if a == QtWidgets.QMessageBox.Yes: mySketch.delConstraint(indexConstraint) FreeCAD.ActiveDocument.recompute

return

if __name__ == '__main__': main procEnd