Files
1993eg1 4d43af5108 Hole guide: UNC and UNF tap drills show in inches (#15684)
* Hole guide: UNC and UNF tap drills show in inches

Since #10369 the Hole dialog shows UNC and UNF tap drills in inches (1/4-20 UNC reads 0.201 in); hovering the box gives the millimetre values. Metric and pipe sizes still show millimetres. Updated the Tap drill diameter example, Try it step 5 and the tip about checking the drill. Checked on v0.40.1.

* Hole guide: hover shows the tap maker's drill, not the typed one

   Per CodeRabbit: hovering Tap drill diameter always shows the catalogue drill in millimetres and the accepted range, even after a different drill is typed. Kept the "type it in" instruction.
2026-11-12 22:43:23 +00:00

6.6 KiB
Raw Permalink Blame History

Put a hole in a solid body: a simple hole, a counterbore, a countersink or a tapped hole. You set the location, size, depth and drill point, the same things a print calls out.

Before you start

  • You need a solid body with a face to drill into. The hole goes straight into the face. A single hole can go on a flat or curved face; locating it from edges needs a flat face.
  • Locate the hole from edges of that face, the same way a print dimensions a hole from two edges. Pick an edge as Reference 1 and type its distance, then do the same for Reference 2. Both edges must be straight and must not be parallel to each other: pick one side edge and one front or back edge, not two opposite sides.
  • To drill several holes at once, sketch a point for each hole on the face first. Then open Hole, set Placement to Multiple and select the points you want. Only the points you select get a hole.

Options

Choice in the dialog Meaning Example or reason to choose it
Personal Presets Saves the dialog settings under a name you choose (Save new), so you can reuse them. Presets are saved in your profile, so they carry over to every design. Rename and Delete manage saved presets. Save a "1/4-20 blind" preset once and pick it for every tapped hole of that size.
Placement Single drills one hole on the face you pick. Multiple drills a hole at each sketch point you select. Single for one hole located from edges. Multiple for a bolt pattern laid out in a sketch.
Face The face the hole is drilled into. Click the top face of the part.
Reference 1 and Distance 1 An edge of the face, and how far the hole center is from it. The left edge, 0.75 in.
Reference 2 and Distance 2 A second edge, and how far the hole center is from it. The front edge, 0.75 in.
Extents How the depth is set. Distance drills to the Depth you type. Use Distance for a blind hole.
Hole Type Simple is a straight hole. Counterbore and Countersink add a bore or a cone at the top. Counterbore for a socket head cap screw. Countersink for a flat head screw: 82° for inch screws, 90° for metric.
Hole Tap Type Simple is a plain drilled hole with a Diameter you type. Tapped drills the tap drill size and shows the thread settings. Choose Tapped for any tapped hole.
Profile (Tapped) The thread standard. UNC for coarse inch threads, UNF for fine inch threads.
Size (Tapped) The thread size, from a list. The Designation box shows the callout. 1/4-20 UNC.
Tap drill diameter (Tapped) The drill for the tapped hole. It fills in the standard tap drill for the size, the one on a tap drill chart (the app's messages call it "the tap maker's drill"), and you can type a different one. The app accepts drills from the smaller of the thread's minor diameter and the standard tap drill, up to 5% over the standard tap drill, and says the allowed range if you go outside it. For a custom metric size with no entry in the app's tap drill table, the app fills in major diameter minus pitch, the usual rule of thumb; check a tap drill chart. 1/4-20 UNC fills in 0.201 in (a #7 drill); hover the box to see 5.105 mm. Typing 0.203 in (13/64) is accepted; 0.220 in is refused because too little thread would engage.
Full thread depth (Tapped) On: the thread runs the full depth of the hole. Off: a Thread depth box appears. Turn it off for a blind tapped hole.
Thread depth (Tapped) How deep the full thread goes, separate from the drill Depth. Drill 0.625 in deep with 0.50 in of thread, so a standard tap doesn't bottom out.
Hand (Tapped) Right or Left. Right unless the print calls for LH.
Modeled (Tapped) On: the thread groove is cut into the hole wall. Off: the thread is carried as a callout only. Leave it off unless you need to see the thread or 3D print it. A modeled thread makes the part slower to rebuild.
End (Modeled on) Square stops the thread sharp at the bottom. Fade runs it out over a length, the way a tap's chamfered end leaves it. Fade for a realistic blind tapped hole.
Drill Point The bottom of the hole. Angle leaves a drill point. Use Angle for a hole made with a twist drill.
Depth How deep the hole goes. Measured to the end of the full diameter, not the tip of the drill point.
Tip Angle The angle of the drill point. Default is 118°. 118° for a standard jobber drill. 135° for most carbide and split-point drills.
Diameter (Simple) The drill size for a plain hole. Type the drill size, such as 0.201 in.

Try it: a 1/4-20 tapped hole 0.75 in from two edges

  1. Click New Sketch and choose the XY plane. Draw a 2-point rectangle from the origin, 3 in × 2 in. Click Finish Sketch.
  2. Click Extrude and set the distance to 0.75 in. Click OK.
  3. Click Hole, then click the top face.
  4. Click Reference 1, pick the left edge of the top face and set Distance 1 to 0.75 in. Click Reference 2, pick the front edge and set Distance 2 to 0.75 in.
  5. Set Hole Tap Type to Tapped, Profile to UNC and Size to 1/4-20 UNC. Check that Tap drill diameter shows 0.201 in.
  6. Turn off Full thread depth. Set Depth to 0.625 in and Thread depth to 0.50 in. Click OK.

Tips and common mistakes

  • Do locate holes from edges the way the print dimensions them. When the part changes size, the holes keep their distances from those edges.
  • Do use Tapped and pick the size from the list instead of typing a drill diameter. The hole then carries the thread callout, and the tap drill comes from a standard tap drill chart.
  • Do check the Tap drill diameter before clicking OK. UNC and UNF sizes show it in inches; metric and pipe sizes show millimetres. If your shop runs a different drill, such as 0.203 in for 1/4-20 in steel, type it in. Hovering over the box shows the tap maker's drill in millimetres and the accepted range, not the drill you typed.
  • Don't turn on Modeled just to show the hole is tapped. The callout already says it.
  • Do turn off Full thread depth on blind tapped holes and set a Thread depth shorter than the drill Depth, so a standard tap doesn't bottom out.
  • Do type the unit with the number when the print is in another unit. In a millimetre design, typing 0.75 in enters 19.05 mm.
  • Don't expect every hole to work on sheet metal. Sheet metal holes must go straight into a flat panel; holes into the edge of the sheet, countersinks and drill points are refused there.

See also

{{#command solid.thread}} cuts a thread on any round face, including the outside of a shaft. {{#command solid.pattern.circular}} repeats a hole around a center for a bolt circle. {{#command solid.chamfer}} breaks the edge of a hole.