着脱式ケーブルトレイ

着脱式プローブホルダーにオシロスコープのプローブをセットしたときに垂れ下がったケーブルを受ける、ケーブルトレイも着脱式で作ってみました。
import FreeCAD as App
import Draft

# パラメーター
wt = 1.6   #肉厚
filletR = 2 #フィレット半径
fillet2R = wt*0.49  #フィレット(小)半径
fillet3R = filletR + wt #フィレット(大)半径
sizeX = 120  #外形(x)
sizeY = 30  #外形(y)
sizeZ = 25  #外形(z)
bsPosX = [(15+(30*i)) for i in range(4)]   #着脱ソケット位置(x)
bsSizeX = 10    #着脱ベース底部幅/2
bsSizeY = 3     #着脱ベース厚み
bsSizeZ = 20    #着脱ベース高さ
bsGrdXZ = 1/10  #着脱ベース斜面の傾き(x/z)
bsGrdXY = 1/1   #着脱ベース斜面の傾き(x/y)
bsfilletR = 0.5 #着脱ベース部フィレット半径
scSizeX = bsSizeX + wt  #着脱ソケット幅/2
scSizeY = 3 + wt    #着脱ベース厚み
scfilletR = 0.2 #着脱ソケット部フィレット半径

def box(
    body,   #追加先ボディ
    name = 'Box',   #名前
    size = (10, 20, 30),    #サイズ
):
    feature = App.ActiveDocument.addObject('PartDesign::AdditiveBox', name)
    feature.Length = size[0]
    feature.Width = size[1]
    feature.Height = size[2]
    b = body.addObject(feature)
    doc.recompute()
    return b[0]

#加算ロフト
def aloft(
    body,
    sections,
    name = 'AdditiveLoft'
):
    lf = body.newObject('PartDesign::AdditiveLoft',name)
    lf.Profile = sections[0]
    lf.Sections += sections[1:]
    for s in sections:
        s.Visibility = False 
    return lf

#加算ロフトによる多面体
def aloft_hedron(
    body,
    l_vertices, #頂点リスト[[]]
    name = 'alhedron'
):
    l_w = [Draft.make_wire([App.Vector(p) for p in lp], closed=True) for lp in l_vertices]
    [body.addObject(w) for w in l_w]
    lf = aloft(body, l_w, name)
    return lf

#ブーリアン演算
def pd_boolean(
    body,   #演算を受けるボディ
    l_obj,  #演算するボディ
    type = 'Fuse',
    name = 'Boolean',
):
    bl = body.newObject('PartDesign::Boolean', name)
    bl.addObjects(l_obj)
    bl.Type = type
    for o in l_obj:
        o.Visibility = False 
    return bl

# 厚みツール
def thickness(
    body,
    shape,  #適用対象図形
    face,
    name = 'Thickness',
    wth = 1 #厚み
):
    th = body.newObject('PartDesign::Thickness', name)
    th.Base = shape, face
    th.Value = wth
    return th

# 押し出し
def pad(
    body,
    profile,
    name = 'Pad',
    len = 10    #押し出し長
):
    pd = body.newObject('PartDesign::Pad', name)
    pd.Profile = profile
    pd.Length = len
    if type(profile) != list:
        profile.Visibility = False
    return pd


doc = App.activeDocument()
if doc == None:
    #アクティブドキュメントが存在しなければ新規作成
    doc = App.newDocument()


#着脱ベース
for i in range(2):  #0:肉抜きなし 1:あり
    bd_bs = doc.addObject('PartDesign::Body',f'base{i}')
    x = sizeX + (30 * (i+1))
    bx0 = x - bsSizeX
    bx1 = x + bsSizeX
    xdy = bsSizeY * bsGrdXY  #背面と内側のxサイズの差
    xdz = bsSizeZ * bsGrdXZ  #上下のxサイズの差
    bz0 = 0
    bz1 = bsSizeZ
    l2_p = [
        [(bx0+xdy, 0, bz0), (bx1-xdy, 0, bz0), (bx1-xdz-xdy, 0, bz1), (bx0+xdz+xdy, 0, bz1)]
        ,[(bx0, bsSizeY, bz0), (bx1, bsSizeY, bz0), (bx1-xdz, bsSizeY, bz1), (bx0+xdz, bsSizeY, bz1)]
    ]
    bs = aloft_hedron(bd_bs, l2_p, f'pg{i}')
    doc.recompute()

    #肉厚分の箱にくり抜く
    if i > 0:
        faces = bs.Shape.Faces
        bf = [f'Face{i+1}' for i,f in enumerate(faces) if (bsSizeY-0.1) < f.CenterOfMass.y < (bsSizeY+0.1)]
        bs = thickness(bd_bs, bs, bf, f'bs_ol{i}', wt)
        doc.recompute()

    #フィレット
    edges = bs.Shape.Edges
    fil_edges = []
    for i, ed in enumerate(edges):
        sel = False
        for vx in ed.Vertexes:
            if (
            ((0+0.1) < vx.Y)
            ):
                sel = True
                break
        if sel:
            fil_edges.append(f'Edge{i+1}')
    fil = bd_bs.newObject('PartDesign::Fillet',f'bsfil{i}')
    fil.Radius = bsfilletR
    fil.Base = (bs, fil_edges)
    doc.recompute()


#ケーブルトレイのボディ
bd_ct = doc.addObject('PartDesign::Body','cabletray')

#外形の箱
ct = box(bd_ct, 'outline', (sizeX, sizeY, sizeZ))

#肉厚分の箱にくり抜く
faces = ct.Shape.Faces
bf = [f'Face{i+1}' for i,f in enumerate(faces) if (sizeZ-0.1) < f.CenterOfMass.z < (sizeZ+0.1)]
ct = thickness(bd_ct, ct, bf, 'box_ol', wt)
doc.recompute()

#着脱ソケット用に背面の厚みを増やす
faces = ct.Shape.Faces
bf = [f'Face{i+1}' for i,f in enumerate(faces) if (wt-0.1) < f.CenterOfMass.y < (wt+0.1)]
ct = pad(bd_ct, [ct, bf],'socketwall', (bsSizeY))

#着脱ソケット
for i, x in enumerate(bsPosX):
    bd_sc = doc.addObject('PartDesign::Body',f'socket{i}')
    bx0 = x - bsSizeX
    bx1 = x + bsSizeX
    xdy = bsSizeY * bsGrdXY #背面と内側のxサイズの差
    xdz = sizeZ * bsGrdXZ   #上下のxサイズの差
    bz0 = 0
    bz1 = sizeZ
    l2_p = [
        [(bx0+xdy, 0, bz0), (bx1-xdy, 0, bz0), (bx1-xdz-xdy, 0, bz1), (bx0+xdz+xdy, 0, bz1)]
        ,[(bx0, bsSizeY, bz0), (bx1, bsSizeY, bz0), (bx1-xdz, bsSizeY, bz1), (bx0+xdz, bsSizeY, bz1)]
    ]
    sc = aloft_hedron(bd_sc, l2_p, f'sc{i}')
    ct = pd_boolean(bd_ct, [bd_sc], 'Cut', f'bsc{i}')
doc.recompute()

#フィレット(大)
edges = ct.Shape.Edges
fil_edges = []
for i, ed in enumerate(edges):
    sel = False
    if (
        ((sizeY-0.1) < ed.CenterOfGravity.y < (sizeY+0.1)) and
        (((sizeZ/2)-0.1) < ed.CenterOfGravity.z < ((sizeZ/2)+0.1))
    ):
        sel = True
        fil_edges.append(f'Edge{i+1}')
fil = bd_ct.newObject('PartDesign::Fillet','Fillet')
fil.Radius = fillet3R
fil.Base = (ct, fil_edges)
doc.recompute()
ct = fil

#フィレット
edges = ct.Shape.Edges
fil_edges = []
for i, ed in enumerate(edges):
    sel = False
    for vx in ed.Vertexes:
        if (
         ((wt-0.1) < vx.Z < (wt+0.1))
        ):
            sel = True
            break
    if sel:
        fil_edges.append(f'Edge{i+1}')
fil = bd_ct.newObject('PartDesign::Fillet','Fillet')
fil.Radius = filletR
fil.Base = (ct, fil_edges)
doc.recompute()
ct = fil

#フィレット(小)
edges = ct.Shape.Edges
fil_edges = []
for i, ed in enumerate(edges):
    sel = False
    for vx in ed.Vertexes:
        if (
         ((wt+0.1) < vx.Z) and (bsSizeY < vx.Y)
        ):
            sel = True
            break
    if sel:
        fil_edges.append(f'Edge{i+1}')
fil = bd_ct.newObject('PartDesign::Fillet','Fillet')
fil.Radius = fillet2R
fil.Base = (ct, fil_edges)
doc.recompute()
ct = fil

##着脱ソケット部のフィレット
edges = ct.Shape.Edges
fil_edges = []
for i, ed in enumerate(edges):
    sel = False
    for vx in ed.Vertexes:
        if (
         #着脱ソケット部
         (((0-0.1) < vx.Y < (bsSizeY+0.1)) and ((0+0.1) < vx.Z))
        ):
            sel = True
            break
    if sel:
        fil_edges.append(f'Edge{i+1}')
fil = bd_ct.newObject('PartDesign::Fillet','Fillet')
fil.Radius = scfilletR
fil.Base = (ct, fil_edges)
doc.recompute()
ct = fil