Macro Shake Sketch

Description

Shake a sketch in order to discover its unconstrained parts.

Enter edit mode for a sketch and launch the macro. The macro will add a random displacement on all sketch points. The sketch is then solved, constrained parts will retain their position, free parts will move. Always run this macro on a copy of the original sketch.

Restore the original Sketch with the Undo (Ctrl+Z) and Redo (Ctrl+Y) button (labeled "Shake Sketch") or be careful working on a copy of your file because the macro "dismantles all" to display and you may need to start over.

Install

Available in Addon manager, or manual install.

Script

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Macro Shake_Sketch.py

# -*- coding: utf-8 -*-

# FreeCAD macro to shake a sketch in order to discover its unconstrained parts.
#
# A Gaussian noise is introduced in all sketch points and the sketch is then
# solved.
# Beware that the sketch can look different because some constraints have
# several solutions. In this case, just undo.
#
# This file is released under the MIT License.
# Author: Gaël Ecorchard v1.0 & v1.1
# Author: heda v1.2
# Version:
# - 1.3: 2022-06-01
#       * added openTransaction(u"Shake Sketch") for restore the original Sketch
# - 1.2: 2021-10-22
#       * made macro runnable for current versions of fc
#       * added Part.LineSegment
#       * added start info & result dialogue
#       * hides constraints during shake
#       * added simple debug printing
# - 1.1: 2014-10-31
#       * correct import for Part
# - 1.0: 2014-08
#       * first release
# Amplitude of the point displacements.
# The standard deviation of the Gaussian noise is the largest sketch dimension
# multiplied by this factor.

__title__ = 'Sketch Shaker'
__version__ = '1.3'
__date__ = '2022/06/01'
__icon__ = 'https://wiki.freecad.org/images/4/4a/Macro_Shake_Sketch.png'

displacement_amplitude = 0.1
debug_print = False

# End of configuration.

from random import gauss

from PySide.QtGui import QMessageBox

import FreeCADGui as Gui
from FreeCAD import Base
import Part

print('Running Macro ' + __title__ + ' ver: ' + __version__)
FreeCAD.ActiveDocument.openTransaction(u"Shake Sketch")    # memorise les actions (avec annuler restore)

# For each sketch geometry type, map a list of points to move.
g_geom_points = {
    Base.Vector: [1],
    Part.Line: [1, 2],  # first point, last point
    Part.LineSegment: [1, 2],  # first point, last point
    Part.Circle: [0, 3],  # curve, center
    Part.ArcOfCircle: [1, 2, 3],  # first point, last point, center
} # moves bsplines and conics via lines and circles, no op for Part.Points


def dprint(msg, *args):
    if debug_print:
        if args:
            print(msg.format(*args))
        else:
            print(msg)

class BoundingBox:
    xmin = xmax = ymin = ymax = None

    def enlarge_x(self, x):
        if self.xmin is None:
            self.xmin = self.xmax = x
        elif self.xmin > x:
            self.xmin = x
        elif self.xmax < x:
            self.xmax = x

    def enlarge_y(self, y):
        if self.ymin is None:
            self.ymin = self.ymax = y
        elif self.ymin > y:
            self.ymin = y
        elif self.ymax < y:
            self.ymax = y

    def enlarge_point(self, point):
        self.enlarge_x(point.x)
        self.enlarge_y(point.y)

    def enlarge_line(self, line):
        self.enlarge_x(line.StartPoint.x)
        self.enlarge_x(line.EndPoint.x)
        self.enlarge_y(line.StartPoint.y)
        self.enlarge_y(line.EndPoint.y)

    def enlarge_circle(self, circle):
        self.enlarge_x(circle.Center.x - circle.Radius)
        self.enlarge_x(circle.Center.x + circle.Radius)
        self.enlarge_y(circle.Center.y - circle.Radius)
        self.enlarge_y(circle.Center.y + circle.Radius)

    def enlarge_arc_of_circle(self, arc):
        # TODO: correctly compute the arc extrema (cf. toShape().BoundBox)
        self.enlarge_x(arc.Center.x)
        self.enlarge_y(arc.Center.y)


def get_sketch_dims(sketch):
    bbox = BoundingBox()
    for geom in sketch.Geometry:
        if isinstance(geom, Base.Vector):
            bbox.enlarge_point(geom)
        elif isinstance(geom, (Part.Line, Part.LineSegment)):
            bbox.enlarge_line(geom)
        elif isinstance(geom, Part.Circle):
            bbox.enlarge_circle(geom)
        elif isinstance(geom, Part.ArcOfCircle):
            bbox.enlarge_arc_of_circle(geom)
    if None in (bbox.xmin, bbox.ymin):
        dprint('sketch bbox not found')
        return 0, 0
    else:
        dprint('sketch bbox found')
        return bbox.xmax - bbox.xmin, bbox.ymax - bbox.ymin


def add_noise(point, sigma):
    """Add a Gaussian noise with standard deviation sigma"""
    dprint('  x0:{:>9.3f}  y0:{:>9.3f}', point.x, point.y)
    point.x = gauss(point.x, sigma)
    point.y = gauss(point.y, sigma)
    dprint('  xt:{:>9.3f}  yt:{:>9.3f}', point.x, point.y)


def move_points(sketch, geom_index, sigma):
    point_indexes = g_geom_points.get(type(sketch.Geometry[i]), [])
    # Direct access to sketch.Geometry[index] does not work. This would,
    # however prevent repeated recompute.
    # not checked validity of comment for v1.2
    moved = False
    for point_index in point_indexes:
        dprint('---- geo idx [{:>3} ] -- pt idx [{:>3} ] ----',
               geom_index, point_index)
        point = sketch.getPoint(geom_index, point_index)
        add_noise(point, sigma)
        try:
            sketch.movePoint(geom_index, point_index, point)
        except ValueError as e:
            dprint(repr(e))
        new_pos = sketch.getPoint(geom_index, point_index)
        test = point.isEqual(new_pos, 0)
        dprint('  did it move? {}', test)
        if test: moved = True
    return moved

def toggle_constraints(sketch, toggle):
    for cid in toggle:
        sketch.toggleVirtualSpace(cid)
    

view_provider = Gui.activeDocument().getInEdit()

shake_it = False
if not view_provider:
    msg = 'A sketch needs to be in edit to be shaken.'
    print(msg)
    _ = QMessageBox.information(None, __title__, msg)
else:
    sketch = view_provider.Object
    if sketch.TypeId == 'Sketcher::SketchObject':
        sketch.recompute() # ensure update
        to_virtual = [cid for cid, cts in enumerate(sketch.Constraints)
                      if cts.InVirtualSpace]
        sketch_span = get_sketch_dims(sketch)
        sigma = max(sketch_span) * displacement_amplitude
        dprint('sketch span: dx:{:>9.3f} dy:{:>9.3f}', *sketch_span)
        dprint('sigma for gauss-dist: {:.3f}', sigma)
        toggle_constraints(sketch, to_virtual)
        msg = ('Shake sketch will deform the loose parts of the sketch.\n'
               'The deformation can be restored with : \n'
               'the Undo (Ctrl+Z) and Redo (Ctrl+Y) button (labeled "Shake Sketch").\n'
               'If that is not desired, click Cancel,\n'
               'and run the macro on a copy of the sketch.\n\n'
               'Visibility of constraints has been toggled.\n'
               'Visibility of constraints is restored'
               ' after shaking the sketch.')
        reply = QMessageBox.information(None, 'Running Macro ' + __title__ + ' ver: ' + __version__, msg,
                                        QMessageBox.Ok | QMessageBox.Cancel,
                                        QMessageBox.Ok)
        shake_it = reply == QMessageBox.Ok
        
        if not shake_it:
            toggle_constraints(sketch, to_virtual)

if shake_it:
    nbr_moves = 0
    for i in range(sketch.GeometryCount):
        did_move = move_points(sketch, i, sigma)
        if did_move:
            nbr_moves += 1

    msg = 'Did {} moves. Sketch has a total of {} geometry entities.\n\n'
    msg = msg.format(nbr_moves, sketch.GeometryCount)
    open_verts = sketch.OpenVertices
    if open_verts:
        if len(open_verts) == 1:
            ov, form = 'one', 'vertex'
        else:
            ov, form = len(open_verts), 'vertices'
        msg += 'Sketch has {} open {}.'.format(ov, form)
        msg += ('\nA sketch with open vertices'
                ' cannot be used to create a solid.')
    else:
        msg += 'Sketch is free from open vertices.'

    msg += ('\n\nMenu: "Sketch/Validate Sketch..." can be used\n'
            'for additional info about sketch status.')
    
    _ = QMessageBox.information(None, 'Running Macro ' + __title__ + ' ver: ' + __version__, msg)
    toggle_constraints(sketch, to_virtual)
        

print('Macro finished.')