mirror of
https://github.com/bherbruck/solidcraft.git
synced 2026-11-19 07:01:00 +00:00
4d43af5108
* 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.
6.6 KiB
6.6 KiB
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
- Click New Sketch and choose the XY plane. Draw a 2-point rectangle from the origin, 3 in × 2 in. Click Finish Sketch.
- Click Extrude and set the distance to 0.75 in. Click OK.
- Click Hole, then click the top face.
- 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.
- 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.
- 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.