FreeCAD macro, creates parametric honeycomb grid, compatible in and out of Part Design

Honeycomb.py

# -*- coding: utf-8 -*-
__version__ = "0.2022.10.26b"

#Honeycomb macro -- creates a feature python parametric honeycomb object for Part Design workbench
#2021, by <TheMarkster> LGPL2.1 or later
import FreeCAD, FreeCADGui, Part
class Honeycomb:
   def __init__(self,obj):
       obj.addExtension("Part::AttachExtensionPython")
       obj.addProperty("App::PropertyFloat","Radius","Honeycomb","Circumradius of the hexagons").Radius = 1
       obj.addProperty("App::PropertyFloat","Separation","Honeycomb","Separation between hexagons").Separation = .5
       obj.addProperty("App::PropertyFloat","Length","Honeycomb","Length of grid").Length = 10
       obj.addProperty("App::PropertyFloat","Width","Honeycomb", "Width of grid").Width = 15
       obj.addProperty("App::PropertyFloat","Height","Honeycomb","Height of grid").Height = 3
       obj.addProperty("App::PropertyBool","EllipticalGrid","Honeycomb","If True, make an elliptical grid of minor diameter = Width, Major Diameter = Length").EllipticalGrid = True
       obj.addProperty("App::PropertyFloatConstraint","XAdjust","Honeycomb","Adjust hexagons in the X direction").XAdjust = (0,-10e4,10e4,.1)
       obj.addProperty("App::PropertyFloatConstraint","YAdjust","Honeycomb","Adjust hexagons in the Y direction").YAdjust = (0,-10e4,10e4,.1)
       obj.addProperty("App::PropertyFloat","BorderOffset","Honeycomb","Offset for border (0 = no border) -1 for inward offset").BorderOffset = 1
       obj.addProperty("App::PropertyFloatConstraint","BorderHeightOffset","Honeycomb","Height Offset for border (0 = same as Height)").BorderHeightOffset = (0.1,-10e4,10e4,.1)
       obj.addProperty("App::PropertyLink","Profile","Honeycomb","Profile, e.g. sketch, to use in place of hexagon, should have radius = 1, centered on origin")
       obj.addProperty("App::PropertyInteger","CountXAdjust","Honeycomb","default: 0 -- amount to add to number of hexagons on X axis")
       obj.addProperty("App::PropertyInteger","CountYAdjust","Honeycomb","default: 0 -- amount to add to number of hexagons on Y axis")
       obj.setEditorMode("Placement",0)
       obj.Proxy = self
       self.fpName = obj.Name

   def makeHexagon(self,radius,origin):
       '''makes a hexagon based on radius and origin, returns it as a wire
       unless a profile is linked to Profile property'''
       fp = FreeCAD.ActiveDocument.getObject(self.fpName)
       if hasattr(fp,"Profile") and fp.Profile:
           profile = fp.Profile
           if not hasattr(profile,"Shape"):
               raise Exception("Invalid profile\n")
           shp = profile.Shape.copy()
           shp.Placement.move(origin)
           shp.scale(radius,origin)
           return shp
       else:
           sin60 = 0.8660254037844386
           tups = [(-1,0,0),(-.5,sin60,0),(.5,sin60,0),(1,0,0),(.5,-sin60,0),(-.5,-sin60,0),(-1,0,0)]
           pts = [FreeCAD.Vector(tup).add(origin) for tup in tups]
           poly = Part.makePolygon(pts).scale(radius,origin)
           return poly

   def makeHoneycomb(self,fp):
       tan15 = 0.2679491924311227
       sin60 = 0.8660254037844386
       yInt = (2 * fp.Radius + fp.Separation - tan15 * fp.Radius)
       xInt = (2 * sin60 * (fp.Radius * 2 + fp.Separation - tan15 * fp.Radius))
       array2XPos = (sin60 * (fp.Radius * 2 + fp.Separation - tan15 * fp.Radius))
       array2YPos = yInt / 2.0
       firstX = fp.Radius
       firstY = fp.Radius
       countX = round(fp.Width/xInt) + 1
       countY = round(fp.Length/yInt) + 1
       if hasattr(fp,"CountXAdjust"):
           countX += fp.CountXAdjust
           countY += fp.CountYAdjust
       vectors = []
       for xx in range(-1,int(countX)):
           for yy in range(-1,int(countY)):
               vectors.append(FreeCAD.Vector(firstX + xx * xInt, firstY + yy * yInt, 0)+FreeCAD.Vector(fp.XAdjust,fp.YAdjust,0))
       array = [self.makeHexagon(fp.Radius, v) for v in vectors]
       array.extend([self.makeHexagon(fp.Radius, v  + FreeCAD.Vector(array2XPos,array2YPos,0)) for v in vectors[:-int(countY+1)]])
       hexagons = Part.makeCompound(array)
       hex_faces = Part.makeFace(hexagons,"Part::FaceMakerCheese")
       if not fp.EllipticalGrid:
           rectTups = [(0,0,0),(fp.Width,0,0),(fp.Width,fp.Length,0),(0,fp.Length,0),(0,0,0)]
           rect_pts = [FreeCAD.Vector(tup) + FreeCAD.Vector(-firstX,0,0) for tup in rectTups]
           rect = Part.makePolygon(rect_pts)
           rect_face = Part.makeFace(rect,"Part::FaceMakerCheese")
           cut = rect_face.cut(hex_faces)
           cut.translate(-cut.BoundBox.Center)
           cut = cut.extrude(cut.Face1.normalAt(0,0).normalize() * fp.Height)
           if fp.BorderOffset == 0:
               return cut
           else:
               border = rect_face.makeOffset2D(fp.BorderOffset, join=2, fill=True)
               border.translate(-border.BoundBox.Center)
               border = border.extrude(border.Face1.normalAt(0,0).normalize()*(fp.Height + fp.BorderHeightOffset))
               fuse = border.fuse(cut)
               return fuse
       else:
           if fp.Width >= fp.Length:
               ellipse = Part.Ellipse(FreeCAD.Vector(0,0,0),fp.Width/2,fp.Length/2).toShape()
           else:
               ellipse = Part.Ellipse(FreeCAD.Vector(0,0,0),fp.Length/2,fp.Width/2)
               plm = FreeCAD.Placement()
               plm.Rotation = FreeCAD.Rotation(FreeCAD.Vector(0,0,1),90)
               ellipse.rotate(plm)
               ellipse = ellipse.toShape()
           ellipse_face = Part.makeFace(ellipse,"Part::FaceMakerCheese")
           hex_faces.translate(ellipse_face.BoundBox.Center - hex_faces.BoundBox.Center + FreeCAD.Vector(fp.XAdjust, fp.YAdjust, 0))
           cut = ellipse_face.cut(hex_faces)
           cut = cut.extrude(cut.Face1.normalAt(0,0).normalize() * fp.Height)
           if fp.BorderOffset == 0:
               return cut
           else:
               if fp.Width >= fp.Length:
                   ellipse_offset = Part.Ellipse(FreeCAD.Vector(0,0,0),fp.Width / 2 + fp.BorderOffset, fp.Length / 2 + fp.BorderOffset).toShape()
               else:
                   ellipse_offset = Part.Ellipse(FreeCAD.Vector(0,0,0),fp.Length / 2 + fp.BorderOffset, fp.Width / 2 + fp.BorderOffset)
                   ellipse_offset.rotate(plm)
                   ellipse_offset = ellipse_offset.toShape()
               ellipse_offset_face = Part.makeFace(ellipse_offset,"Part::FaceMakerCheese")
               if fp.BorderOffset > 0:
                   border = ellipse_offset_face.cut(ellipse_face)
               else:
                   border = ellipse_face.cut(ellipse_offset_face)
               border = border.extrude(border.Face1.normalAt(0,0).normalize()*(fp.Height + fp.BorderHeightOffset))
               fuse = border.fuse(cut)
               return fuse

   def execute(self,fp):
       shape = self.makeHoneycomb(fp)
       fp.positionBySupport()
       shape.Placement = fp.Placement

       #shape.transformShape(fp.Placement.inverse().toMatrix(), True)
       if hasattr(fp,"AddSubShape"):
           fp.AddSubShape = shape
       if hasattr(fp,"BaseFeature") and fp.BaseFeature:
           full_shape = shape.fuse(fp.BaseFeature.Shape)
           full_shape.transformShape(fp.Placement.inverse().toMatrix(),True)
           fp.Shape = full_shape
       else:
           fp.Shape = shape


class HoneycombVP:

   def __init__(self, obj):
       '''Set this object to the proxy object of the actual view provider'''
       obj.Proxy = self

   def attach(self, obj):
       '''Setup the scene sub-graph of the view provider, this method is mandatory'''
       self.Object = obj.Object

   def updateData(self, fp, prop):
       '''If a property of the handled feature has changed we have the chance to handle this here'''
       # fp is the handled feature, prop is the name of the property that has changed
       pass

   def getDisplayModes(self,obj):
       '''Return a list of display modes.'''
       modes=[]
       modes.append("Flat Lines")
       return modes

   def getDefaultDisplayMode(self):
       '''Return the name of the default display mode. It must be defined in getDisplayModes.'''
       return "Flat Lines"

   def setDisplayMode(self,mode):
       '''Map the display mode defined in attach with those defined in getDisplayModes.\
               Since they have the same names nothing needs to be done. This method is optional'''
       return mode

   def onChanged(self, vp, prop):
       '''Here we can do something when a single property got changed'''
       #FreeCAD.Console.PrintMessage("Change property: " + str(prop) + ""+chr(10))

   def claimChildren(self):
       return []

   def setupContextMenu(self, vobj, menu):
       pass

   def setEdit(self,vp,modNum):
       pass

   def onDelete(self, vobj, subelements):
       if hasattr(vobj.Object,"_Body") and vobj.Object._Body: #do this only when the object is in a PD body
           #need to ensure the next feature in the tree's BaseFeature property points to our BaseFeature
           solids = [feat for feat in vobj.Object._Body.Group if feat.isDerivedFrom("PartDesign::Feature") and feat.BaseFeature == vobj.Object]
           if len(solids) == 1: #found previous solid feature
               solids[0].BaseFeature = vobj.Object.BaseFeature
       return True

   def getIcon(self):
       '''Return the icon in XPM format which will appear in the tree view. This method is\
               optional and if not defined a default icon is shown.'''
       XPM = '''
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};
'''
       return XPM

   def __getstate__(self):
       '''When saving the document this object gets stored using Python's json module.\
               Since we have some un-serializable parts here -- the Coin stuff -- we must define this method\
               to return a tuple of all serializable objects or None.'''
       return None

   def __setstate__(self,state):
       '''When restoring the serialized object from document we have the chance to set some internals here.\
               Since no data were serialized nothing needs to be done here.'''
       return None



if __name__ == "__main__":

    import os
    import FreeCAD, FreeCADGui, Part
    if ".FCMacro" in __file__ and not os.path.exists(__file__.replace(".FCMacro",".py")):
        current = __file__
        new_name = current.replace(".FCMacro", ".py")
        with open(new_name, "w") as new_file:
            with open(__file__, "r") as current_file:
                new_file.write(current_file.read())
        FreeCAD.Console.PrintWarning("A new file has been created named Honeycomb.py in order for Honeycomb objects to work when you reload a document containing a Honeycomb object.\n")
    from Honeycomb import Honeycomb, HoneycombVP
    doc = FreeCAD.ActiveDocument if FreeCAD.ActiveDocument else FreeCAD.newDocument()
    fp = doc.addObject("PartDesign::FeatureAdditivePython","Honeycomb")
    Honeycomb(fp)
    HoneycombVP(fp.ViewObject)
    selx = FreeCADGui.Selection.getSelection()
    if selx:
        profile = selx[0]
        if hasattr(profile,"Shape"):
            fp.Profile = profile
    body=FreeCADGui.ActiveDocument.ActiveView.getActiveObject("pdbody")
    if body:
        body.addObject(fp)