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Holes

Design's Hole (Shift+H, with a sketch selected on a body that has a solid) drills at every circle centre and lone point of the sketch, construction geometry left out. With no sketch selected and a flat face of the solid clicked, it drills where you clicked, from a hidden sketch of its own on that face; add points to that sketch for more holes. It starts as a custom hole the size of the sketch's circles (the most common size when they differ, which the log says; 5 mm for a sketch of points alone), 10 mm deep, drilled against the sketch's normal; Reversed drills the other way. The task panel sets the rows below; a script sets the same fields by name (pc.design.hole, pc.design.set).

A plate cut through four holes: plain, a socket head counterbore, a countersink, and a modeled M8 thread with its drill point

Size

Standard is Custom (a plain diameter) or a thread standard:

Standard Sizes Form
ISO metric coarse, fine M1.6 to M48, M3x0.35 to M36x3 60°
UNC #1 to 1 inch 60°
UNF #0 to 1 inch 60°
UNEF #12 to 1 inch 60°
BSW 1/8 to 1 inch 55°
BSF 3/16 to 1 inch 55°
BSP parallel (G) 1/16 to 2 55°
BSP taper (Rc) 1/16 to 2 55°, 1:16 taper
NPT 1/16 to 2 60°, 1:16 taper

A sized hole drills the tap drill when Threaded (tap drill) is on, otherwise the clearance of its Fit (close, normal, loose: ISO 273 for metric sizes, ASME B18.2.8 for unified ones; the other standards drill the major diameter), or Custom, a clearance diameter of your own. A tapped taper thread drills the thread's minor diameter at the face and narrows 1:16 on the diameter from there.

Class is the internal thread's class: 4H to 8H and 4G to 8G for metric (a G class moves the diameters out by the ISO 965-1 allowance, (15 + 11 P) µm), 1B to 3B for unified, Medium or Normal for Whitworth. Pipe threads have none. Left-hand thread turns a modeled thread the other way.

Modeled thread (offered once Threaded is on) cuts the thread itself into the wall, for printing it rather than tapping it: the standard's flank angle, out to its major diameter, along a cone for a taper thread. Thread length is Depth given (the Thread depth row), the Whole hole, or the hole Less the run-out of three pitches a tap leaves at the bottom. A through hole threaded its whole length (or less the run-out, which a through hole has none of) runs as far as the solid reaches along the hole's axis, out past the far side.

Cosmetic thread (on a threaded hole that is not modeled) keeps the bore at its tap drill and shows the thread instead: a helix of the thread's pitch down the bore, as far as the hole goes (a through hole's to where it leaves the solid), and the designation in its row's tooltip in the tree ("Hole · M6 thread"). The designation is also a callout at each bore's mouth under View › Annotations, a column of the Assembly's parts list ("2 × M6 thread") and of its CSV, and a callout (its text and its leader) in a STEP export, naming the bore it threads so a reader puts it on that part. No groove reaches an export: drill the tap size, print, and tap the hole afterwards.

A mirror or pattern of the hole, or of the whole body, threads each copy it makes the same way, cut to the same hand across a mirror, and counts it in the parts list and the export. A copy that lands off the material is not threaded. A path pattern's and a fill pattern's copies are not threaded yet, since only the built solid says where they fall.

Depth and bottom

Through all or a Depth. A blind hole's Drill point is flat or angled (118°, 135° or any Point angle from 10° to 170°); Point within the depth makes the depth run to the tip rather than to the end of the wall. Taper leans the wall in toward the bottom, up to 44° either way (a tapped taper thread uses its own).

Start at is where drilling starts: the sketch's own plane, a datum plane, another sketch's plane or a flat face of the solid (click it, then pick Selected face), the circles carried along the drill to it. A face is found again on the solid before the hole, so the hole follows it when the features before it change. Start offset starts that much further into the material, or above it when negative.

While the task is open, two handles in the view stand on the first centre of the sketch: one drags Start offset along the drill and the other the Depth (none for a hole through all). They work as every feature's view handles do; see View handles under Design features in EDITING.md.

Hole cut

The seats below are offered only for a hole sized from an ISO metric thread, and a size the seat's table lacks says so in the panel.

Nut trap

Nut trap cuts a hexagonal pocket at one end of the hole that holds a nut captive, beside any hole cut. It is sized from the nut of the hole's ISO metric thread; PRINTING.md has the sizes, the clearance, the depth and the side it sits on. A hole sized otherwise takes a nut trap of its own size.

For printing

The Printing section shapes a hole for the printer.

Shape is the bore's outline across its axis:

The point faces the body's +Z, the build direction, unless you choose another axis. The shape is the drill's, and a counterbore's, spotface's or counterdrill's bore takes it too; a countersink and a drill point stay round. A hole drilled along its up direction has no side for a point, and says so. A mirror or a pattern turns the point with the copy.

Bridge layer leaves a thin layer (0.2 mm by default, a layer or two) across the hole at the floor of its counterbore, spotface, countersink or counterdrill. Printed with the cut facing down, the cut's floor is then one bridge across its whole width rather than a ring hanging round the hole. Drill the layer out after printing. A hole with no cut has no floor to bridge, and says so.

pc.design.hole{sketch = s, diameter = 5, through_all = true, shape = "Teardrop"}
pc.design.hole{sketch = s, diameter = 3.4, through_all = true, bridge = 0.2,
  cut = {Counterbore = {diameter = 6.5, depth = 3.4}}}

shape is "Round", "Teardrop" or "FlatTop", or a table for more: shape = {FlatTop = {angle_deg = 40, up = {0, 1, 0}}}.

Your own cuts

Cuts you use often go in hole_cuts.json in the application's configuration folder (~/.config/printcad/ on Linux, beside settings.json). It is read once a run, the first time a hole lists its cuts; its profiles are listed under the standard cuts, and picking one copies its sizes into the hole. Screw seats and None are left out of it, since a seat needs the hole's size.

{
  "profiles": [
    { "name": "M3 heat insert", "cut": { "Counterbore": { "diameter": 4.2, "depth": 5.0 } } },
    { "name": "Deburr 6", "cut": { "Countersink": { "diameter": 6.0, "angle_deg": 90.0 } } },
    { "name": "Stepped 8", "cut": { "Counterdrill": { "diameter": 8.0, "depth": 3.0, "angle_deg": 118.0 } } },
    { "name": "Face 12", "cut": { "Spotface": { "diameter": 12.0, "depth": 0.5 } } }
  ]
}

Scripts

pc.design.hole{
  sketch = s,
  depth = 8,
  thread = {standard = "Unc", size = "1/4-20", class = "3B", left_handed = false},
  threaded = true,
  drill_point = {Angled = {angle_deg = 118}},
  cut = {Counterdrill = {diameter = 9, depth = 2, angle_deg = 90}},
}

standard is one of IsoMetricCoarse, IsoMetricFine, Unc, Unf, Unef, Bsw, Bsf, BspParallel, BspTaper or Npt; size is the designation the panel lists. A size alone, thread = "M6" or thread = "1/4-20", takes the first standard that has it. A drill point is drill_point = {Angled = {angle_deg = 135}}, or {Angled = {}} for 118°. A screw seat is cut = {Seat = {seat = "SocketHead"}}, or "Countersunk", "ButtonHead", "SlottedCountersunk", "CrossCountersunk", "LowHeadCap", "CapScrewWithWasher", "HexHead". clearance sets a clearance of your own. modeled_thread = true cuts the thread (with threaded = true), its length from thread_length, "Given" (with thread_depth in mm), "HoleDepth" or "RunOut"; cosmetic_thread = true (on a threaded hole, modeled_thread off) shows the thread instead, the bore left at its tap drill. nut_trap = true adds a nut trap at the mouth; a table sets it: nut_trap = {side = "Bottom", clearance = 0.4, depth = 3, across_flats = 7, turn_deg = 30, standard = "Din934"}, each field left out taking its usual value. start = {offset = 2, at = plane} starts it 2 mm in from a datum plane or a sketch; start = {face = {point = {x, y, z}, normal = {0, 0, 1}}} from a face. face_point = {x, y, z} and face_normal in place of sketch place one hole on a flat face at that point.

Holes already in a solid

Recognize holes (pc.design.recognize_holes) turns the round bores of a body's solid, imported ones included, into Hole features: their faces go in one Delete faces feature, and each set of alike holes on one plane is drilled again from a hidden sketch of their centres. Bores it cannot describe (counterbores, countersinks, slots) stay as they are.

Threads on a face

Thread (Design's subtractive group) cuts a thread into a round face the solid already has: a bolt's shank, the outside of a jar's neck, the inside of a cap, or a bore no Hole made. Click the face and choose Thread; which way the face faces tells an external thread from an internal one. The task panel shows what it found (a shaft or a bore, its diameter and length) and sets:

The groove is the same as a modeled hole thread's: the standard's flank angle, flat a pitch's eighth wide at its root, swept along a helix about the face's axis and kept within the face's length, so a thread running the whole of a shank stops square at the head's face rather than cutting into it. A face that is not a cylinder fails on the feature.

pc.design.thread{body = body, face_point = {5, 0, 8}, face_normal = {1, 0, 0},
  thread = "M10", full_length = false, length = 12, chamfer = true}

thread = "Custom" with pitch and depth cuts a thread of your own.

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