Drilling and hole making
For a hole the same size as your bit, drill it with a peck cycle. For a bigger hole, helical interpolate or pocket it, which gives a better hole and lets one bit make any size. Plunging an end mill straight down is the option that breaks tools.
Three ways to make a hole
| Method | How | Best for | Watch out for |
|---|---|---|---|
| Drilling | Plunge straight down, usually pecking in stages | Holes the same size as the tool, shelf pins, dowels | Chips have nowhere to go. Peck. |
| Helical interpolation | The tool spirals down and around the hole wall | Any hole larger than the tool. The best surface finish. | Needs CAM support, and a tool smaller than the hole |
| Pocketing a circle | Treat the hole as a round pocket | Large holes, when helical is not available | Leaves a small scallop at the centre if the tool is not centre cutting |
Helical interpolation is the quietly superior option most hobby users never use. One 1/8 inch bit can cut a 0.3 inch hole, a 0.5 inch hole and a 1 inch hole, all with good walls, with no tool change.
Pecking
A peck cycle plunges a short distance, retracts to clear chips, and goes back in deeper. It exists because a blind hole is the worst possible case for chip evacuation: there is exactly one exit and the tool is in it.
- Peck depth is commonly set around one bit diameter per peck in wood, less in deep holes.
- Full retract versus partial retract. A full retract clears completely and takes longer. A partial retract, sometimes called chip breaking, is faster and clears less.
- Deep holes need smaller pecks. The deeper you go, the harder it is for chips to travel out.
Drills versus end mills
A twist drill is designed to plunge: it has a point that cuts at the centre and flutes shaped to bring chips straight up. An end mill mostly is not. Many end mills have very little cutting ability at the exact centre, which is why plunging one feels like pushing rather than cutting.
Hole size accuracy
A helically interpolated or pocketed hole comes out slightly undersize if the tool deflects, and slightly oversize if there is runout. For holes that have to fit something:
- Cut a test hole in scrap and measure it before committing.
- Leave a small allowance and take a finishing pass at full depth.
- Remember that a drilled hole is exactly the bit diameter plus runout, and cannot be adjusted.
Through holes and breakout
Where a hole exits the bottom face, the last bit of material has nothing supporting it and it blows out. Two fixes: a sacrificial backer under the workpiece, or stopping just short and cutting the last bit with a slower plunge.
Shelf pin and repeated hole patterns
This is where a CNC genuinely beats a jig. A line of perfectly spaced, perfectly aligned holes is trivial for the machine and fiddly by hand. Draw the pattern once, and the accuracy is the machine's problem forever after.