Hole
Drill simple, counterbored, countersunk or tapped holes at the points of a sketch, with screw, bolt, dowel and thread sizes.
- Hole HPart Studio toolbar
| SchoolCAD | Onshape | Fusion | SOLIDWORKS |
|---|---|---|---|
| Hole | Hole | Hole | Hole Wizard |
Hole drills real workshop holes into a part: screw holes, bolt holes, dowel holes, cable holes and threaded (tapped) holes. You put a point in a sketch where each hole goes, then pick the size from a list, such as 8g screw, countersunk (4.5 mm) or 8 mm dowel hole, 20 deep. One Hole feature can drill lots of holes at once.
How to use it#
- Start a sketch on the face the holes go into. Use Point (.) to put a point where each hole goes, and add dimensions to put the points in the right place. Finish the sketch.
- Click Hole, or press H. The newest sketch with points is chosen for you.
- Choose a Preset, or choose the hole type and type your own sizes.
- For a hole with a depth, drag the arrow at the bottom of the hole, or type the Depth.
- Check the preview, then click ✓ or press Enter.
Options#
| Option | What it does |
|---|---|
| Sketch | The sketch with the points. It says how many holes it will make. |
| Preset | Workshop sizes for screws, dowels, bolts, a cable hole, shelf pins and tapped holes (M3 to M12). It starts on 8g screw, countersunk (4.5 mm). |
| Simple | A plain, straight hole. |
| Counterbore | A wider, flat-bottomed recess for a bolt head. Set the Recess Ø and Recess depth. |
| Countersink | A cone, so a countersunk screw sits flush. Set the Head Ø and the Angle. |
| Tapped | A hole with a screw thread, for a bolt or machine screw (M1.6 to M24). Choose the Thread: the hole is drilled at the tap drill size (Tap drill Ø) and the thread goes as deep as the Thread depth. Normally the thread is cosmetic: it is shown on engineering drawings, as in Onshape and SOLIDWORKS, not modelled as a real spiral. |
| Pitch | Advanced only, for M6 and up: the coarse pitch (the usual one) or a fine pitch (ISO 261), such as M8 × 1. The tap drill changes to suit. |
| Modelled thread (for 3D printing) | Advanced only: the real thread is cut into the hole wall (the ISO 60° profile), so a 3D-printed part takes a real bolt. Leave it off for parts made in the workshop: there the tap cuts the thread. |
| Print fit | With a modelled thread: extra room in the thread, in mm, so a 3D print does not bind on the bolt. 0.1 to 0.3 mm suits most printers. |
| Hand | Advanced only: Right hand (almost every screw) or Left hand (the left pedal of a bike, gas fittings). |
| Diameter | The size of the hole, in mm. |
| Depth | How deep it goes, in mm. Tick Through all to go right through. |
| Start | Sketch plane measures the depth from the sketch. Where it meets the part measures each hole from where it meets the part, so holes in a curved or sloping face all end up the same depth. |
| ⇅ Flip direction | Drills the other way. |
| Drill into | Tick the parts to drill. With nothing ticked, it drills every part it meets. |
Tips#
- Change any size and the preset becomes Custom size.
- A circle in the sketch works as well as a point: the hole goes at its centre. The size of the circle does not matter, only the Diameter in the dialog.
- Hole finds its own way into the part. If the holes would miss, it tries the other way.
- The arrow only shows for a hole with a depth, measured from the Sketch plane. When you drag it, the steps get smaller as you zoom in. Hold Shift for finer steps, or press Esc to put the depth back.
- Where it meets the part suits curved faces, like the deck of a surf handplane.
- For a row of holes, put several points in one sketch, or make one hole and use Pattern.
- To change a hole later, double-click inside it on the model, or double-click it in the feature tree.
- A modelled thread makes the part much heavier (thousands of triangles), so tick it last, once the design is done. To thread a hole made another way, or a round shaft, use Thread.
If it does not work#
- First make a sketch on the face and put a Point (or a circle) where each hole goes.
- The sketch has no points or circles to put holes on. Add a point (or a circle) where each hole goes. The end of a line does not count: a hole needs a point of its own, or the centre of a circle.
- The cut did not remove anything. Check the direction, depth or the part it cuts. The points may not be over the part, or the sketch may be on the wrong face.
- The holes miss the part. Put the sketch points over the part (looking along the hole), or flip the direction. This one comes with Where it meets the part.
- The hole is as wide as an M6 thread, so no thread is modelled. A modelled thread needs the hole drilled at the tap drill size: choose the thread again and the Tap drill Ø goes back to it.