Aluminum drilling settings depend on the alloy condition and the drill design. Walter’s 2024 holemaking guide lists different cutting speeds for five nonferrous material groups and two named solid-carbide drill families at a drilling depth of 3 × the drill diameter. The table keeps those conditions together so a speed from one material or tool is not accidentally applied to another. Walter describes the figures as average standard values and directs users to its GPS system for final cutting data.
Aluminum and light metal drilling data
Walter solid-carbide drilling data for selected aluminum alloys
Walter 3×Dc starting data for two named solid-carbide drill families across five aluminum material groups. Feed is the Walter VRR chart index, not mm/rev.
1–10 of 10 matching rows (10 total)
Free engineering resource
Unlock CSV downloads and printing
Enter your email to download the displayed table page as CSV or print it.
CSV and print access for this browser session
Submit the form to unlock CSV downloads and printing.
Search and sort apply to all 10 rows. Print and CSV include only the 10 rows shown on this page.
How to read the values
The Walter material groups separate wrought aluminum from cast aluminum, then distinguish hardenable condition and silicon content. N1 is non-hardenable wrought aluminum; N2 is hardened, hardenable wrought aluminum. N3 and N4 are cast aluminum with up to 12% silicon, in non-hardenable and hardened conditions. N5 is cast aluminum above 12% silicon. The hardness and tensile-strength columns describe the guide’s representative material categories, not acceptance limits for every alloy in the group.
The cutting speed is in metres per minute. The second drill column identifies a product family: DC260 Advance or DC180 Supreme. The source’s VRR value is a feed-rate chart index, not a feed per revolution. It should not be entered as mm/rev or multiplied by RPM as though it were a physical feed value. The catalog lists emulsion or oil as cutting media and marks minimum-quantity lubrication or dry machining as possible for these entries.
Calculating a spindle-speed starting point
For a 6 mm DC180 drill in N1 material, the catalog speed is 472 m/min. Using n = 1000vc/(πD), with vc in m/min and D in mm, gives about 25,000 rpm. This is a kinematic conversion of the catalog speed, not an instruction that every machine should run at that speed. Check spindle limits, runout, workholding, tool overhang, coolant delivery and the drill manufacturer’s current recommendations before setting the machine.
Hole depth matters. These figures are presented for 3 × Dc drilling. A deeper hole can change chip evacuation and heat removal, so a speed/feed chosen for the listed depth should not be assumed suitable for deep-hole work. Use an appropriate drilling cycle and the tool supplier’s data when the application goes beyond the table’s conditions.
Choosing the correct material row
Do not select a group from the word “aluminum” alone. Identify the actual alloy, whether it is wrought or cast, its heat-treated condition and relevant hardness. Silicon content changes the cutting behavior of cast alloys, and a hardened grade can differ from a soft wrought material. If the certificate or drawing does not provide enough information to map the workpiece to the guide, ask the material supplier or tooling engineer instead of guessing.
The two drill families have different listed speeds for several cast-alloy groups. That is why the tool column is part of each row. Do not transfer the DC180 value to another drill, coating, diameter range or geometry merely because the tool is also carbide. Check whether the selected size falls in the catalog range and whether the machine can supply the required coolant and speed.
Limits and safe application
These are toolmaker starting references rather than guaranteed production parameters. Actual performance also depends on alloy chemistry, casting skin, hardness variation, machine rigidity, tool condition, entry geometry and chip evacuation. Walter identifies the catalog data as average standard values. A validated process should be developed for the actual workpiece and equipment, with inspection of tool wear, burrs, hole size and surface finish.
Keep the feed-rate chart index distinct from feed per revolution, and use the correct material group and drill series. For the worked example, 6 mm and 472 m/min give approximately 25,000 rpm; a feed rate still needs the applicable manufacturer chart or tool-specific calculation. This reference does not establish a safe operating window or replace the current Walter GPS recommendation for a particular job.
Source and scope
Data source: Walter Technical Compendium — Holemaking (2024), B1 drilling from solid, 3×Dc data. Walter identifies the values as average standard values and recommends selecting final cutting data with Walter GPS.
