Macro Sketch Constraint From Spreadsheet

Description
'''Work in progress. It works for me. Tell me if anything is wrong.'''

Macro which, with a simple click on a spreadsheet cell, adds a length constraint to a line or between 2 points using a spreadsheet cell alias or address (ex. C2). Future changes to the spreadsheet will update the constraint. The macro can create alias for you.

Just select 1 line, 2 points or a constraint, click on a spreadsheet cell and run the macro. You can select lines, points at the ends of a line, points, circles or arcs of circles.



Usage
If you run the macro and have not yet created a spreadsheet, the macro suggests to create one and then opens it so that you can start filling it.



It is not mandatory, but it is better to use aliases in your spreadsheet. The macro can create aliases from texts in cells.



1) Select:
 * a line,
 * two points (end of a line, center of a circle, etc.)
 * or a length constraint.



2) Click on a spreadsheet cell, with or without an alias, that has a numerical value:



3) Run the macro.

4) Select the desired type of constraint:



If the cell has an alias, the length property of the constraint will be something like 'Spreadsheet.alias'. Otherwise, something like 'Spreadsheet.D4'.



5) If the constraint causes a conflict in the sketch and the "conflict detection" box is checked, the macro will offer to delete the new constraint:



If you select an existing constraint, you can change its value for a value from a spreadsheet:



The macro can also handle external geometry from another sketch:

To make things even more refined, if, for example, a line is horizontal rather than vertical, when the dialogue box opens, the focus will be on the button for apply a horizontal constraint. If the line is vertical rather than horizontal, the focus will be on the button to apply a vertical constraint. In both cases, simply press the enter key if you are happy with this choice.



Links

 * Forum discussion (French)
 * Macros recipes
 * How to install macros
 * How to customize toolbars

Credits
Thanks to openBrain, mario52 and onekk for their help on the code! Thanks to Syres	for tests and for the help on the format in the code. Thanks to Roy043 and David69 for the various reviews and improvements to the wiki.

Script
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Code
ver 00.02.41 25/03/2023 by 2cv001 Macro_Sketch_Constraint_From_Spreadsheet.FCMacro

__author__ = "2cv001" __title__  = "Macro Sketch Constraint From Spreadsheet" __date__   = "2023/03/25"    #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'],["'",],['?',],['"',],['(',],[')',],['#',],                 ['$',],['+',],['-',],['*',],['/',],['\\',] ]
 * 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.

def remplaceCartatParEquivalent(caractere): caracResult = caractere for couple in caracEquivalents: if (couple[0] == caractere): caracResult = couple[1] break return caracResult
 * 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 True 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 isExistObjectType(type) : def firstObject(doc = App.ActiveDocument): for obj in doc.Objects: if obj.TypeId == type: return obj return None myObject = firstObject if not myObject : if type == 'Spreadsheet::Sheet' : messageText = "No spreadsheet in your document. Create one ?" objectName = 'SpreadSheet'
 * 1) Test if an object of a type exist and ask for a creation if not.
 * 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

elif type == 'PartDesign::Body' : messageText = "No Body in your document. Create one ?" objectName = 'Body' wantNewObjet = QtWidgets.QMessageBox.question(None, "object not detected",       messageText, QtWidgets.QMessageBox.Yes | QtWidgets.QMessageBox.No) if wantNewObjet == QtWidgets.QMessageBox.Yes: myObject = App.activeDocument.addObject(type, objectName) myObject.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 : a = QtWidgets.QMessageBox.question(None, "",           "No document find. Create one ? ",            QtWidgets.QMessageBox.Yes | QtWidgets.QMessageBox.No, QtWidgets.QMessageBox.No) if a == QtWidgets.QMessageBox.Yes : App.newDocument if a == QtWidgets.QMessageBox.No: return existBodyNew = isExistObjectType ('PartDesign::Body') in ['no', 'new'] existSpreadSheetNew = isExistObjectType ('Spreadsheet::Sheet') in ['no', 'new'] if existBodyNew or existSpreadSheetNew : return
 * 1) Main proceddure
 * 1) Main proceddure

# 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

# 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'] )) :

# 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' # ask the user what kind of constraint he wants #       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