How does the Drilling Toolpath work in VCarve Pro & Aspire, including peck drilling for deep holes?

Overview

The Drilling Toolpath drives a drill bit straight down into the material to a specified depth at the center of each selected closed vector. It's the fastest and most reliable way to cut holes when you need precise hole positioning for dowels, hardware inserts, shelf pins, registration pins, or any application where a circular pocket isn't necessary. There are no X/Y cutting moves, just vertical plunges, so it is faster than a pocket or profile for a large number of holes. It is available in both VCarve Pro and Aspire.

How the Software Determines the Drill Position

The software drills at the center of each selected closed vector, regardless of the vector's size or shape. This means:

• A circle: drills at the circle's center
• A square, rectangle, or other closed shape: drills at the shape's center

Important: The Drilling toolpath does NOT cut the circumference of the circle. It plunges the selected tool at the center point, so the hole diameter equals the bit diameter, not the vector diameter. To drill a 1/4" hole, use a 1/4" bit. The circle diameter only matters for the Vector Selector filter. For larger holes use Profile Inside or a Pocket toolpath (see below).

Setup Steps

1. Draw circle vectors for each hole position
2. Select all circle vectors for this drilling operation
3. Open Drilling Toolpath (Toolpaths tab)
4. Set Start Depth: usually 0 (from the material surface). Enter the pocket depth if drilling into the bottom of an existing pocket
5. Set Cut Depth: how deep to drill, relative to the Start Depth. Total hole depth = Start Depth + Cut Depth
6. Select your drill from the Tool Database. The Tool Database lets you specify the drill diameter and cutting parameters
7. Choose peck drilling settings (see below)
8. Click Calculate

Regular Drilling vs Peck Drilling

Regular Drilling (no peck): The tool plunges straight to the full Cut Depth. Suitable for shallow holes in soft materials like foam or MDF where chip packing is not a problem.

Peck Drilling: The drill cuts to a shallow depth, retracts to clear chips, plunges again to the next increment, and repeats until full depth. It helps with overheating and breakage. Use it for deeper holes, hardwood, and any precision hole where chip packing could make the bit wander or break. A common rule of thumb is to peck any hole deeper than about one bit diameter.

How to enable peck drilling:

1. Check Use Peck Drilling in the Drilling Toolpath form
2. The peck depth is the Pass Depth set for the drill in the Tool Database, so set it there before running. If the Pass Depth is larger than the Cut Depth, the hole is drilled in one cycle. For example, a 1" Cut Depth with a 0.25" Pass Depth is drilled in 4 cycles
3. Choose a retract style:

Two Retract Modes

Retract above cutting start: The tool retracts fully out of the hole after each peck. The Retract Gap (R) is a fixed distance above the start cut depth. This is best for clearing chips completely, but the retract and plunge distances grow as the hole deepens, so machining time is longer.

Retract above the height of the previous pass: Instead of retracting out of the hole, the tool retracts to a height relative to the previous peck depth. The Retract Gap (R) is the distance above the previous pass. The retracts are the same size for every peck, so it is typically faster, but it will not necessarily clear the chips completely.

Dwell at the bottom of each drill pass: Optionally pauses the drill at the bottom of each peck before retracting. The Dwell Time is measured in seconds. Your post-processor must support the Dwell section and may need updating.

Controlling Drill Order

By default, the software optimizes the order to reduce machining time. To drill in a specific order:

1. Check Use Vector Selection Order in the toolpath form
2. Select the hole vectors in the order you want them drilled
3. Calculate. The drill follows your selection sequence

Using End Mills for Drilling (Plunge Milling)

When a dedicated drill bit isn't available, an end mill can plunge-mill holes:

• Use a center-cutting end mill (most 2-flute end mills are center-cutting)
• Plunge rate is the feed that applies, since the tool is only moving in Z. Start with a reduced plunge rate for hardwoods and test on scrap
• A plunged end mill leaves a flat-bottomed hole, unlike a drill's angled point
• For clean round holes, follow with a Profile toolpath using a circle vector of the same diameter

When NOT to Use the Drilling Toolpath

Hole larger than your drill bit: The Drilling toolpath only drills a hole equal to the bit diameter. For larger holes, use:

• Profile Inside toolpath: the bit orbits around the inside of the circle to cut a clean hole. Use it for clean through-holes in panels.
• Pocket toolpath: removes all material inside the circle. Good for blind holes.

Tip for cleaner holes with a router: Some users prefer a slightly oversized circle with a Profile Inside toolpath using a spiral ramp entry. The ramp descent can produce a cleaner hole interior than a straight plunge. Good for visible holes such as shelf pins in hardwood.

Vector Selector Tip for Drilling

The Vector Selector is especially useful with the Drilling toolpath. In the toolpath form, use the Vector Selection section and choose Only Circles with a specific diameter. This creates an automatic selection filter so the toolpath always selects exactly the circles you intend to drill, even when the design is updated. It also saves well in toolpath templates for repeat jobs.

Toolpath templates: Drilling is a good candidate for templates because hole diameters are consistent across jobs (shelf pin = always 5mm, dowel = always 1/4", etc.). Save a "5mm shelf pin drill" template, load it into a new cabinet job, and the shelf pin holes are auto-selected.

Practical Applications

• Shelf pin holes: Regularly spaced circles on a cabinet side, all the same depth
• Dowel joinery: Matching hole patterns on two mating parts
• Hardware inserts: Confirmat screws, barrel nuts, Euro screws. Drill to spec before assembly
• Registration pins: Drill matching pin holes in the spoilboard and material for two-sided machining flip registration

Common Mistakes

• Expecting the circle diameter to determine hole size: the bit diameter determines hole size
• Not enabling peck drilling on deep holes: chip packing can cause breakage
• Setting the Retract Gap too small: with Retract above the height of the previous pass and a very small Retract Gap, the drill barely lifts between pecks and chips are not cleared
• Leaving Project toolpath onto 3D Model checked by accident when a 3D model exists in the job: the drill depths follow the model surface instead of the flat material surface