diff --git a/Documentation/README.md b/Documentation/README.md
index 0a89ff4..c8704b9 100644
--- a/Documentation/README.md
+++ b/Documentation/README.md
@@ -8,6 +8,7 @@ This is the documentation for the tools included in the _FusedFilamentDesign_ ad
| |  | [**Thread Forming Ribs**](./ffDesign_RibThreads.md) | Hole geometry for rib thread forming |
| |  | [**Teardrop Shape**](./ffDesign_Teardrop.md) | Teardrop-shaped holes for better horizontal holes and to avoid seam inaccuracy |
| |  | [**Roof Bridge**](./ffDesign_RoofBridge.md) | Roof bridges for horizontal holes |
+| |  | [**Hex Nut Hole**](./ffDesign_HexNut.md) | Hexagonal recess at the end of a hole to capture a hex nut |
|  | | [**Zip Tie Channels**](./ffDesign_ZipTieChannels.md) | Generate parametric zip tie channels on a part's surface |
|  | | [**Auto Fillet**](./ffDesign_AutoFillet.md) | Automatically add fillets to vertical edges |
diff --git a/Documentation/ffDesign_HexNut.md b/Documentation/ffDesign_HexNut.md
new file mode 100644
index 0000000..ac2916b
--- /dev/null
+++ b/Documentation/ffDesign_HexNut.md
@@ -0,0 +1,62 @@
+
+## Command: Hex Nut Hole
+This command cuts a hexagonal recess at one end of a hole, so that a hex nut
+can be captured inside the part. This is useful for embedding nuts in printed
+parts without a press fit.
+
+## Prerequisites
+- A [PartDesign Hole][pd-hole] feature must be selected or the tip of the
+ active body must be a [PartDesign Hole][pd-hole].
+
+## Usage
+Run this command to generate a hex nut recess for the selected Hole feature. A
+dialog will open in the [Task Panel][task-panel] where you can control the
+generation.
+
+- **Hex Nut Size**: The distance between two opposite flat sides of the hex
+ nut, also known as the spanner size. This is the nominal dimension of a hex
+ nut, not the radius to a corner.
+- **Hex Hole Depth**: The depth of the hexagonal recess, measured from the
+ selected face.
+- **Start on the opposite face**: When checked, the recess starts on the
+ opposite face of the part instead of on the hole entry face. The tool
+ determines the location of this face from the shape of the part.
+- **Rotate by 30 degrees**: When checked, the hexagon turns
+ by 30 degrees. A vertex then points where a flat side faces in the default
+ orientation. A regular hexagon looks the same after a 60 degree turn, so 30
+ degrees is the useful angle.
+
+Click "OK" to then proceed generating the recess. This will create the
+following features:
+
+- A pocket for the hex nut recesses of all holes in this Hole feature. When
+ the recess starts on the opposite face, each hole gets its own pocket.
+
+Additionally, two properties will be added to the original Hole feature which
+can be used to parametrically control the recesses:
+
+- `HexNutSize` is the distance across the flats of the hex nut.
+- `HexNutDepth` is the depth of the hexagonal recess.
+
+## Parametricity
+This feature is parametric with respect to the following variables:
+
+- Hole
+ * The position of the circles in the supporting sketch of the original Hole feature.
+ * The position of the supporting sketch itself.
+- Hex Nut Properties of the Hole
+ * Hex nut size (`HexNutSize` property)
+ * Hex nut recess depth (`HexNutDepth` property)
+
+This feature is **not** parametric with respect to the following variables.
+You will need to delete the feature and recreate it to update these variables:
+
+- Supporting Sketch
+ * The number of circles in the supporting sketch of the original Hole feature.
+- Hole
+ * The direction of the hole (`Reversed` property).
+ * The choice between the hole entry face and the opposite face.
+ * The rotation of the hexagon (vertex up or side up).
+
+[pd-hole]: https://wiki.freecad.org/PartDesign_Hole
+[task-panel]: https://wiki.freecad.org/Task_panel
diff --git a/Documentation/ffDesign_HoleWizard.md b/Documentation/ffDesign_HoleWizard.md
index dad3c98..959d9da 100644
--- a/Documentation/ffDesign_HoleWizard.md
+++ b/Documentation/ffDesign_HoleWizard.md
@@ -8,6 +8,7 @@ selecting one of the following tools:
- [ Thread Forming Ribs](./ffDesign_RibThreads.md)
- [ Teardrop Shape](./ffDesign_Teardrop.md)
- [ Roof Bridge](./ffDesign_RoofBridge.md)
+- [ Hex Nut Hole](./ffDesign_HexNut.md)
## Prerequisites
- A [PartDesign Hole][pd-hole] feature must be selected or the tip of the
diff --git a/InitGui.py b/InitGui.py
index b34948b..630e82d 100644
--- a/InitGui.py
+++ b/InitGui.py
@@ -6,6 +6,7 @@
import ffDesign_RibThreads
import ffDesign_Teardrop
import ffDesign_RoofBridge
+import ffDesign_HexNut
import ffDesign_ZipTieChannels
import ffDesign_AutoFillet
diff --git a/README.md b/README.md
index 17ee812..0726907 100644
--- a/README.md
+++ b/README.md
@@ -6,7 +6,7 @@ This is a [FreeCAD PartDesign][fc-partdesign] addon for FFF/FDM 3D-printing desi

## Installation
-This addon is available through the [FreeCAD Addon-Manager](https://wiki.freecad.org/Std_AddonMgr).
+This addon is available through the [FreeCAD Addon-Manager][addon-manager].
## Usage
The addon adds a new toolbar to the [PartDesign][fc-partdesign] workbench where the new tools can be accessed. Check the tooltips for guidance.
@@ -26,12 +26,13 @@ To find out more about using the tools included in this addon, please check the
| |  | **Thread Forming Ribs** | Hole geometry for [rib thread forming][df3dp-ribthreads] (**R5.4**) |
| |  | **Teardrop Shape** | Teardrop-shaped holes for [better horizontal holes][df3dp-horizontal-holes] and to avoid [seam inaccuracy][df3dp-seam] (**R2.2** & **R2.3**) |
| |  | **Roof Bridge** | Roof bridges for [horizontal holes][df3dp-horizontal-holes] (**R2.2**) |
+| |  | **Hex Nut Hole** | Hexagonal recess at the end of a hole to capture a hex nut |
|  | | **Zip Tie Channels** | Generate parametric [zip tie channels][df3dp-zip-ties] on a part's surface (**R4.1**) |
|  | | **Auto Fillet** | Automatically add [fillets on all vertical edges][df3dp-vertical-fillets] of a part. (**R2.1**) |
| _Planned_ | | **Seam Groove** | Generate a seam groove to control [where the slicer will place the perimeter seams][df3dp-seam] (**R2.3**)|
| _Planned_ | | **Sacrificial Layer** | Generate a [sacrificial layers][df3dp-sacrificial] for some surface with holes (**R3.4**) |
-(The **R#.#** numbers reference the rules from my [Design for 3D-Printing][df3dp-main] guide)
+(The **R#.#** numbers reference the rules from my [Design for 3D-Printing][df3dp-main] guide).
## Changelog
To follow updates of this addon, please check the [Releases Page](https://github.com/Rahix/FusedFilamentDesign/releases) or the [CHANGELOG](./CHANGELOG.md) file.
@@ -39,6 +40,7 @@ To follow updates of this addon, please check the [Releases Page](https://github
## License
This addon is licensed under the `LGPL-2.1-or-later` license. See [LICENSE](./LICENSE) for more info.
+[addon-manager]: https://wiki.freecad.org/Std_AddonMgr
[fc-partdesign]: https://wiki.freecad.org/PartDesign_Workbench
[fc-hole]: https://wiki.freecad.org/PartDesign_Hole
[fc-additional-workbenches]: https://wiki.freecad.org/How_to_install_additional_workbenches
diff --git a/Resources/icons/ffDesign_HexNut.svg b/Resources/icons/ffDesign_HexNut.svg
new file mode 100644
index 0000000..5c47272
--- /dev/null
+++ b/Resources/icons/ffDesign_HexNut.svg
@@ -0,0 +1 @@
+
\ No newline at end of file
diff --git a/Resources/panels/ffDesign_HexNut.ui b/Resources/panels/ffDesign_HexNut.ui
new file mode 100644
index 0000000..37576aa
--- /dev/null
+++ b/Resources/panels/ffDesign_HexNut.ui
@@ -0,0 +1,98 @@
+
+
+ HexNutDialog
+
+
+
+ 0
+ 0
+ 400
+ 190
+
+
+
+ Hex Nut Hole
+
+
+
+
+
+ Hex Nut Size
+
+
+
+
+
+
+ mm
+
+
+ 0.000000000000000
+
+
+ Distance between two opposite flat sides of the hex nut (spanner size).
+
+
+
+
+
+
+ Hex Hole Depth
+
+
+
+
+
+
+ mm
+
+
+ 0.000000000000000
+
+
+ Depth of the hexagonal recess, measured from the hole's entry face.
+
+
+
+
+
+
+ Start the hexagonal recess on the opposite face of the part instead of on the hole entry face.
+
+
+ Start on the opposite face
+
+
+
+
+
+
+ Turn the hexagon by 30 degrees, so don't have to print a bridge.
+
+
+ Rotate by 30 degrees
+
+
+
+
+
+
+ The hexagonal recess extends from the selected face into the part.
+
+
+ true
+
+
+
+
+
+
+
+ Gui::QuantitySpinBox
+ QWidget
+ gui::quantityspinbox.h
+
+
+
+
+
diff --git a/Resources/panels/ffDesign_HoleWizard.ui b/Resources/panels/ffDesign_HoleWizard.ui
index a283592..1b1c78f 100644
--- a/Resources/panels/ffDesign_HoleWizard.ui
+++ b/Resources/panels/ffDesign_HoleWizard.ui
@@ -7,7 +7,7 @@
00400
- 320
+ 380
@@ -162,6 +162,35 @@ Preconditions:
+
+
+
+
+ 0
+ 0
+
+
+
+ Add a hexagonal recess to the end of the hole to hold a hex nut.
+
+
+ Add Hex Nut Hole
+
+
+
+ icons:ffDesign_HexNut.svgicons:ffDesign_HexNut.svg
+
+
+
+ 32
+ 32
+
+
+
+ Qt::ToolButtonStyle::ToolButtonTextBesideIcon
+
+
+
diff --git a/ffDesign_HexNut.py b/ffDesign_HexNut.py
new file mode 100644
index 0000000..912f744
--- /dev/null
+++ b/ffDesign_HexNut.py
@@ -0,0 +1,264 @@
+import math
+
+from PySide import QtCore
+
+import FreeCADGui as Gui
+import FreeCAD as App
+import Part
+import Sketcher
+
+import ffDesign_Utils as Utils
+
+
+HEX_SIDES = 6
+
+
+def make_parametric_hex_nut(
+ sketch,
+ *,
+ hole_loc: Utils.LocationExprSet,
+ size_expr: str,
+ rotation: float = 0.0,
+):
+ Utils.assert_sketch(sketch)
+
+ last_geo_id = len(sketch.Geometry)
+ points = []
+ for i in range(HEX_SIDES):
+ angle = 2 * math.pi / HEX_SIDES * i + rotation
+ points.append(App.Vector(math.cos(angle), math.sin(angle), 0))
+
+ new_geo = [Part.LineSegment(points[i], points[(i + 1) % HEX_SIDES]) for i in range(HEX_SIDES)]
+ sketch.addGeometry(new_geo, False)
+
+ new_constraints = []
+ for i in range(HEX_SIDES):
+ new_constraints.append(
+ Sketcher.Constraint("Coincident", last_geo_id + i, 2, last_geo_id + (i + 1) % HEX_SIDES, 1)
+ )
+ sketch.addConstraint(new_constraints)
+
+ # Fix every vertex directly. Equal sides plus points on a circle also
+ # allows a collapsed hexagon, so all vertices get their own coordinates.
+ x = hole_loc.x_expr
+ y = hole_loc.y_expr
+ # The size is across the flats, so the corners sit on a circle of radius
+ # half the flat distance divided by cos(30 degrees), i.e. size / sqrt(3).
+ r = f"({size_expr}) / sqrt(3)"
+ vertex_offsets = []
+ for i in range(HEX_SIDES):
+ angle = 2 * math.pi / HEX_SIDES * i + rotation
+ vertex_offsets.append((f"{r} * {math.cos(angle)!r}", f"{r} * {math.sin(angle)!r}"))
+
+ expressions = []
+ for dx, dy in vertex_offsets:
+ expressions.append(f"{x} + ({dx})")
+ expressions.append(f"{y} + ({dy})")
+
+ last_c = len(sketch.Constraints)
+ new_constraints = []
+ for i in range(HEX_SIDES):
+ new_constraints.append(Sketcher.Constraint("DistanceX", last_geo_id + i, 1, 0))
+ new_constraints.append(Sketcher.Constraint("DistanceY", last_geo_id + i, 1, 0))
+ sketch.addConstraint(new_constraints)
+ for i, expr in enumerate(expressions):
+ sketch.setExpression(f"Constraints[{last_c + i}]", expr)
+
+ sketch.recompute()
+
+
+def _get_far_face_offset(body, hole, profile_sketch, hole_loc):
+ """
+ Distance from the profile plane to the opposite face of the part.
+
+ The result is signed along the profile sketch's local Z axis, so it can be
+ used as the attachment offset of a sketch on the opposite face.
+ """
+ Utils.assert_body(body)
+ Utils.assert_hole(hole)
+ Utils.assert_sketch(profile_sketch)
+
+ profile_placement = profile_sketch.Placement
+ normal = profile_placement.Rotation.multVec(App.Vector(0, 0, 1))
+ direction = normal if hole.Reversed else normal * -1
+ entry = profile_placement.multVec(hole_loc.center)
+
+ # The hole axis itself is empty, so probe the material just next to the
+ # hole wall and look for the last point that is still inside the part.
+ radius = hole.Diameter.Value / 2
+ radial_a = direction.cross(App.Vector(1, 0, 0))
+ if radial_a.Length < 1e-6:
+ radial_a = direction.cross(App.Vector(0, 1, 0))
+ radial_a.normalize()
+ radial_b = direction.cross(radial_a)
+ radial_b.normalize()
+
+ bound = body.Shape.BoundBox.DiagonalLength * 2 + 10
+ entry_proj = entry.dot(direction)
+ distances = []
+ for radial in (radial_a, radial_a * -1, radial_b, radial_b * -1):
+ offset = radial * (radius + 0.05)
+ start = entry + offset - direction * (radius + 3)
+ end = entry + offset + direction * bound
+ common = body.Shape.common(Part.makeLine(start, end))
+ if not common.Vertexes:
+ continue
+ far_proj = max(vertex.Point.dot(direction) for vertex in common.Vertexes)
+ distances.append(far_proj - entry_proj)
+
+ if not distances or max(distances) <= 0:
+ raise Utils.ffDesignError(
+ "Could not find the opposite face of this hole. The hex nut recess was not created."
+ )
+
+ distance = max(distances)
+ return distance if hole.Reversed else -distance
+
+
+def _make_hex_nut_pocket(body, hole, hex_sketch, *, reversed, suffix: str = ""):
+ pocket = body.newObject("PartDesign::Pocket", f"{hole.Name}{suffix}")
+ pocket.Profile = (hex_sketch, "")
+ pocket.ReferenceAxis = (hex_sketch, ["N_Axis"])
+ pocket.Reversed = reversed
+ hex_sketch.Visibility = False
+ pocket.setExpression("Length", f"{hole.Name}.HexNutDepth")
+ pocket.Label = f"{hole.Label}{suffix}"
+ pocket.recompute()
+
+
+def make_hex_nuts(
+ body,
+ hole,
+ *,
+ nut_size: App.Units.Quantity,
+ nut_depth: App.Units.Quantity,
+ far_side: bool = False,
+ vertex_up: bool = False,
+):
+ Utils.assert_body(body)
+ Utils.assert_hole(hole)
+
+ # A regular hexagon has 6-fold symmetry, so a 60 degree turn looks the
+ # same. Turning it by 30 degrees is what swaps a flat side and a vertex.
+ rotation = math.radians(30) if vertex_up else 0.0
+
+ nut_size = App.Units.Quantity(nut_size)
+ assert nut_size.Unit.Type == "Length"
+ nut_depth = App.Units.Quantity(nut_depth)
+ assert nut_depth.Unit.Type == "Length"
+
+ if "HexNutSize" not in hole.PropertiesList:
+ hole.addProperty("App::PropertyLength", "HexNutSize", group="FusedFilamentDesign")
+ hole.HexNutSize = nut_size
+
+ if "HexNutDepth" not in hole.PropertiesList:
+ hole.addProperty("App::PropertyLength", "HexNutDepth", group="FusedFilamentDesign")
+ hole.HexNutDepth = nut_depth
+
+ profile_sketch, profile_partial = Utils.get_hole_profile_sketch(hole)
+ hole_locations = Utils.get_sketch_locations(profile_sketch, Utils.get_hole_profile_type(hole), profile_partial)
+
+ if not far_side:
+ hex_sketch = Utils.make_derived_sketch(body, profile_sketch, "_HexNut")
+ for hole_loc in hole_locations:
+ make_parametric_hex_nut(
+ hex_sketch,
+ hole_loc=hole_loc,
+ size_expr=f"{hole.Name}.HexNutSize",
+ rotation=rotation,
+ )
+ _make_hex_nut_pocket(body, hole, hex_sketch, reversed=hole.Reversed, suffix="_HexNut")
+ return
+
+ # Each hole can exit through a face at a different distance, and a sketch
+ # is planar. So on the opposite side, every hole gets its own sketch.
+ offsets = [
+ (hole_loc, _get_far_face_offset(body, hole, profile_sketch, hole_loc)) for hole_loc in hole_locations
+ ]
+ multiple = len(offsets) > 1
+ for i, (hole_loc, offset) in enumerate(offsets):
+ suffix = f"_HexNut{i + 1:03}" if multiple else "_HexNut"
+ hex_sketch = Utils.make_derived_sketch(body, profile_sketch, suffix)
+ hex_sketch.AttachmentOffset = App.Placement(App.Vector(0, 0, offset), App.Rotation())
+ hex_sketch.recompute()
+ make_parametric_hex_nut(
+ hex_sketch,
+ hole_loc=hole_loc,
+ size_expr=f"{hole.Name}.HexNutSize",
+ rotation=rotation,
+ )
+ _make_hex_nut_pocket(body, hole, hex_sketch, reversed=not hole.Reversed, suffix=suffix)
+
+
+class HexNutTaskPanel:
+ def __init__(self, body, hole):
+ Utils.assert_body(body)
+ Utils.assert_hole(hole)
+
+ self.body = body
+ self.hole = hole
+ self.form = Gui.PySideUic.loadUi(Utils.Resources.get_panel("ffDesign_HexNut.ui"))
+
+ self.form.HexNutSize.setProperty("rawValue", 5.5)
+ self.form.HexNutDepth.setProperty("rawValue", 3.0)
+
+ def accept(self):
+ try:
+ nut_size = self.form.HexNutSize.property("value")
+ nut_depth = self.form.HexNutDepth.property("value")
+ far_side = self.form.FarSide.checkState() == QtCore.Qt.CheckState.Checked
+ vertex_up = self.form.VertexUp.checkState() == QtCore.Qt.CheckState.Checked
+
+ Gui.Control.closeDialog()
+
+ try:
+ App.ActiveDocument.openTransaction("Add hex nut hole")
+ make_hex_nuts(
+ self.body,
+ self.hole,
+ nut_size=nut_size,
+ nut_depth=nut_depth,
+ far_side=far_side,
+ vertex_up=vertex_up,
+ )
+ App.ActiveDocument.recompute()
+ except Exception as e:
+ App.ActiveDocument.abortTransaction()
+ raise e from None
+ else:
+ App.ActiveDocument.commitTransaction()
+ except Utils.ffDesignError as e:
+ e.emit_to_user()
+
+ def reject(self):
+ Gui.Control.closeDialog()
+
+
+class HexNutCommand:
+ def GetResources(self):
+ return {
+ "Pixmap": "icons:ffDesign_HexNut.svg",
+ "MenuText": App.Qt.translate("ffDesign", "Add hex nut hole"),
+ "ToolTip": App.Qt.translate(
+ "ffDesign",
+ "Add a hexagonal recess to the end of a hole to hold a hex nut.\n"
+ "1. Select a Hole feature in the active body.\n"
+ "2. Run this command.\n",
+ ),
+ }
+
+ def Activated(self):
+ try:
+ hole = Utils.get_selected_hole()
+ body = Utils.get_active_part_design_body_for_feature(hole)
+
+ dialog = HexNutTaskPanel(body, hole)
+ Gui.Control.showDialog(dialog)
+ except Utils.ffDesignError as e:
+ e.emit_to_user()
+
+ def IsActive(self):
+ return Utils.check_hole_tool_preconditions()
+
+
+Gui.addCommand("ffDesign_HexNut", HexNutCommand())
diff --git a/ffDesign_HoleWizard.py b/ffDesign_HoleWizard.py
index c7047b5..a126d58 100644
--- a/ffDesign_HoleWizard.py
+++ b/ffDesign_HoleWizard.py
@@ -15,6 +15,7 @@ def __init__(self, hole):
self.form.AddRibThreads.clicked.connect(self.addRibThreads)
self.form.AddRoofBridge.clicked.connect(self.addRoofBridge)
self.form.AddTeardropShape.clicked.connect(self.addTeardropShape)
+ self.form.AddHexNutHole.clicked.connect(self.addHexNutHole)
self.updateCommandAvailability()
@@ -28,6 +29,7 @@ def updateCommandAvailability(self):
# The following hole tools are always available
self.form.AddTeardropShape.setEnabled(True)
self.form.AddRoofBridge.setEnabled(True)
+ self.form.AddHexNutHole.setEnabled(True)
def addCounterboreBridges(self):
FreeCADGui.Control.closeDialog()
@@ -45,6 +47,10 @@ def addTeardropShape(self):
FreeCADGui.Control.closeDialog()
FreeCADGui.runCommand("ffDesign_Teardrop")
+ def addHexNutHole(self):
+ FreeCADGui.Control.closeDialog()
+ FreeCADGui.runCommand("ffDesign_HexNut")
+
def accept(self):
FreeCADGui.Control.closeDialog()
diff --git a/ffDesign_Utils.py b/ffDesign_Utils.py
index 6f29b17..30d91a0 100644
--- a/ffDesign_Utils.py
+++ b/ffDesign_Utils.py
@@ -313,6 +313,8 @@ class LocationExprSet:
vector_expr: str
x_expr: str
y_expr: str
+ # Position of the hole in the sketch's local coordinate system.
+ center: App.Vector
def get_sketch_locations(sketch, profile_type, profile_partial=None):
@@ -329,6 +331,7 @@ def try_make_loc_expr_set(index, obj, kind):
vector_expr=f"vector({x_expr}, {y_expr}, 0)",
x_expr=f"{x_expr} * 1mm",
y_expr=f"{y_expr} * 1mm",
+ center=App.Vector(obj.X, obj.Y, 0),
)
if (profile_type & MASK_PROFILE_CIRCLES) != 0:
if obj.TypeId == "Part::GeomCircle":
@@ -337,6 +340,7 @@ def try_make_loc_expr_set(index, obj, kind):
vector_expr=center,
x_expr=f"{center}.x * 1mm",
y_expr=f"{center}.y * 1mm",
+ center=obj.Center,
)
if (profile_type & MASK_PROFILE_ARCS) != 0:
if obj.TypeId == "Part::GeomArcOfCircle":
@@ -345,6 +349,7 @@ def try_make_loc_expr_set(index, obj, kind):
vector_expr=center,
x_expr=f"{center}.x * 1mm",
y_expr=f"{center}.y * 1mm",
+ center=obj.Center,
)
return None