Machine a Part from Raw Stock — Project Guide

🧑‍🔧 Machine a Part from Raw Stock

Field: Manufacturing / Machining

Written and maintained by the PhDino author · Last reviewed 21 September 2026 · Every calculator used here is tested against independent reference values · how PhDino checks its numbers

Weigh your starting stock, dial in the spindle speed and feed for the drill you'll use, then estimate the cycle time of the drilling operation.

Starting a job on a mill, a CNC router or a drill press usually means three checks before the first cut: knowing what you're starting with (stock weight matters for material cost and for whether your vise or fixture can handle it), dialing in the spindle speed and feed for the tool you will actually use, and estimating how long the operation will take.

This guide carries real numbers between steps. The spindle speed you work out for the drill is the speed the cycle-time estimate needs, and the drill's flutes and chip load set the feed per revolution that estimate uses, so the two calculators agree with each other instead of being run in isolation.

🧮 Metal Stock Weight 🧮 CNC Speeds & Feeds 🧮 Drilling Cycle Time

Speed, feed and why the numbers come in several flavors

Cutting speed is how fast the tool's edge travels over the work, in surface feet per minute (SFM). It is a property of the pairing of tool and material, so tool makers publish it. Spindle speed is the same thing expressed as revolutions per minute for a particular diameter, RPM = SFM × 12 ÷ (π × diameter), which is why a bigger tool has to turn slower at the same cutting speed.

Feed has several flavors too. Chip load is the thickness each cutting edge takes per revolution, feed per revolution is chip load times the number of edges, and feed rate is feed per revolution times RPM. A twist drill has two edges, so its feed per revolution is twice its chip load per tooth, and mixing up which flavor a chart quotes is a common way to run a drill at half or double the intended feed.

What you need before you start

The calculators need four facts, and the tool maker's data supplies most of them.

The workpiece material and the tool material. A high-speed-steel drill and a carbide drill run at very different speeds in the same aluminum.
The drill diameter and the number of flutes, two for a standard twist drill.
The recommended cutting speed and feed for that pairing, from the tool maker's data or a machinist's handbook.
The machine's limits. A small mill or drill press may top out at a few thousand RPM, and if the calculated speed exceeds it you run at the maximum and reduce the feed in proportion.

Steps

1🔲Metal Stock Weight
Start with the raw stock you're cutting from: shape, dimensions, length and material. This gives you the weight, useful for material cost, shipping, and whether your workholding can support it.
🧮 Open the Metal Stock Weight calculator
2🛠️CNC Speeds & Feeds
Run this for the tool you are about to use. For drilled holes that is the drill: enter its diameter, two flutes for a standard twist drill, the cutting speed recommended for your drill material and workpiece material (from the tool maker's data), and a chip load per tooth (the feed per revolution divided by the number of flutes). This returns the spindle RPM and feed rate to actually run. Hit "📋 Copy Values" once you have a result: the spindle speed carries straight into the drilling step next.
🧮 Open the CNC Speeds & Feeds calculator
3⏱️Drilling Cycle Time
"📥 Paste Values" fills in the same spindle speed from Step 2. Add the hole depth and the number of holes, and set the feed per revolution to the drill's flutes times its chip load from Step 2, so the feed rate here matches the one Step 2 reported. This returns the cutting time for the operation.
🧮 Open the Drilling Cycle Time calculator

Worked example: twelve 1/4 in holes through an aluminum plate

A mounting plate is cut from aluminum flat bar, 4 in wide, 0.5 in thick and 1.5 ft long. It needs 12 through holes, 1/4 in in diameter, drilled with a standard two-flute high-speed-steel twist drill. The machine can turn at least 3,100 RPM.

Step 1: Weight of the stock

You enter	Value
Stock Shape	Flat / Plate
Diameter / Side / Width	4 in
Thickness / Wall (flat, tube only)	0.5 in
Length	1.5 ft
Material	Aluminum (0.098 lb/in³)

The calculator returns	Value
Weight per Foot	2.352 lb
Total Weight	3.53 lb

A flat bar's cross-section is width × thickness = 2.0 in². At 0.098 lb per cubic inch of aluminum, a foot (12 in) of it holds 2.0 × 12 × 0.098 = 2.352 lb, so 1.5 ft is 3.53 lb. That is light enough for an ordinary vise, and easy to lift onto the table.

The same bar in steel (0.284 lb per cubic inch) would weigh 10.2 lb, nearly three times as much, which is the sort of difference that changes how you fixture a part.

Step 2: Speed and feed for the drill

You enter	Value
Cutting Speed (SFM)	200 SFM
Tool Diameter	0.25 in
Number of Flutes	2
Chip Load per Tooth	0.0025 in/tooth

The calculator returns	Value
Spindle Speed	3,056 RPM
Feed Rate	15.3 IPM

The cutting speed is what the tool maker specifies for the drill and the material. 200 SFM is a plausible figure for a high-speed-steel drill in aluminum, and coated or carbide drills run faster. The calculator turns it into a spindle speed for this diameter: 200 × 12 ÷ (π × 0.25) = 3,056 RPM.

The chip load per tooth is 0.0025 in, so with 2 flutes the drill advances 2 × 0.0025 = 0.0050 in every revolution, and the feed rate is 3,056 × 0.0050 = 15.3 in/min. If your spindle tops out below that speed, run at its maximum and cut the feed in proportion: the feed per revolution stays the same, so the feed rate falls with the RPM.

Step 3: Cycle time for twelve holes

You enter	Value
Hole Depth	0.5 in
Approach/Clearance Distance	0.1 in
Spindle Speed	3,056 RPM
Feed per Revolution	0.005 in/rev
Number of Holes	12

The calculator returns	Value
Feed Rate	15.28 IPM
Time per Hole	0.03927 min
Total Cycle Time	0.4712 min

The spindle speed comes across from step 2, and the feed per revolution is that drill's flutes times its chip load, 0.0050 in/rev. The feed rate the calculator reports, 15.3 in/min, matches step 2's 15.3 in/min, which is the cross-check that both steps describe the same cut.

Each hole travels the 0.5 in of plate plus a 0.1 in approach, 0.6 in, at 15.3 in/min, so 0.0393 min or about 2.4 seconds. Twelve holes come to 0.47 minutes, about 28 seconds of cutting. The holes are 2 diameters deep, shallow enough to drill in one pass; much deeper than a few diameters, chip packing means pecking.

What it adds up to

Half a minute of cutting is only a small part of the real cycle. Loading the part, spot-drilling each hole so the drill starts true, moving between twelve positions, changing tools and deburring all take longer than the drilling itself, so on a short job the true cycle is often several times the cutting time. Use this estimate to compare setups and to spot an unrealistic quote, not to price a job to the second.

Notes & limitations

Surface Finish Estimate, Tap Drill Size, Bolt Circle Pattern, Sheet Metal Bend Allowance, Tolerance Stack-Up, and Press Brake Tonnage are all real, standalone checks for other parts of a job. They didn't get forced into this particular sequence because there's no genuine shared value between them and a drilling setup specifically.
Real-world cycle time also includes tool changes, rapid moves between holes, and peck-drilling retractions on deep holes. See the Drilling Cycle Time article for what this estimate does and doesn't cover.

Mistakes that break drills and ruin holes

Speeds and feeds are unforgiving in both directions, and these are the slips behind most problems.

Using the wrong diameter for the RPM. The same 200 SFM on a 1/2 in drill is 1,528 RPM, half the speed. Recompute for every tool.
Confusing chip load per tooth with feed per revolution. On a two-flute drill they differ by a factor of two.
Feeding too lightly. A drill that rubs instead of cutting heats up, work-hardens some materials and dulls fast, which is worse than a slightly heavy feed.
Feeding too heavily, which packs the flutes and breaks the drill, especially in deep holes.
Skipping cutting fluid or a chip-clearing pause in aluminum, which welds to the tool.
Letting the machine's maximum RPM quietly override the calculation. Note when it does, and lower the feed rate to match.

Safety, and when to ask a machinist

Clamp the work in a vise or fixture, never hold it by hand, wear eye protection, and keep loose sleeves, gloves and long hair away from anything that turns. A drill that catches the work turns it into a spinning blade.

For hard-to-machine materials such as stainless steel or titanium, for tight tolerances, or for holes that are much deeper than a few diameters, the published data of the tool maker and the advice of an experienced machinist beat any calculator. The figures here are a starting point for a first cut, not a guarantee.

Frequently asked questions

Is SFM the same as RPM?

No. SFM is the speed of the cutting edge over the work, RPM is how fast the spindle turns. They connect through the tool's diameter: RPM = SFM × 12 ÷ (π × diameter), so the same SFM means a higher RPM on a smaller tool.

Where do I find the right cutting speed for my material?

From the tool maker's data for your exact tool and material, or from a machinist's handbook. The ranges are wide because coatings, tool material and coolant all move them, so start at the low end of a range for a first cut and adjust from what you hear and see.

Why is a drill's chip load per tooth only half the feed per revolution?

Because it has two cutting edges sharing the advance. A drill that moves 2 × 0.0025 = 0.005 in per turn takes 0.0025 in from each edge, which is the number a milling-style calculator asks for.

What feed per revolution should a 1/4 in drill use?

Drill makers publish it by diameter and material, and for a drill this size it is typically a few thousandths of an inch per revolution. The 0.005 in used here is in that range, but check the chart for your drill.

Why is the estimated cycle time so short?

Because it is cutting time only. It leaves out loading and unloading, rapid moves between holes, tool changes, pecking on deep holes and any inspection, which together often outweigh the cutting itself on a short job.