Calculating spindle speed for gun drilling is the same as for any turning operation. Get this wrong and you will burn up your tool or leave a terrible surface finish. I run these calculations before every job, and after enough setups the numbers become second nature. Here is how I do it.
The RPM Formula and How I Use It
The standard formula for spindle speed is:
RPM = (Cutting Speed x 1000) / (Pi x Diameter)
Where:
- Cutting speed is in meters per minute (m/min)
- Diameter is in millimeters (mm)
If you work in imperial units (surface feet per minute), the formula becomes:
RPM = (SFM x 3.82) / Diameter (in inches)
I keep both versions in my notebook. In practice, I start with the middle of the manufacturer’s recommended cutting speed range for the material, then adjust based on what the chips tell me. If chips come out burnt or discolored, I drop the RPM. If they are too thin and stringy, I bring it up.
Worked Examples
Seeing the numbers on real diameters makes the formula click. Here are the calculations I run most often.
6mm Gun Drill in Mild Steel
Cutting speed: 80 m/min
RPM = (80 x 1000) / (3.14 x 6) = 80,000 / 18.84 = 4246 RPM
I typically round this to 4200 RPM for setup.
10mm Gun Drill in Mild Steel
Cutting speed: 80 m/min
RPM = (80 x 1000) / (3.14 x 10) = 80,000 / 31.4 = 2547 RPM
I set this at 2550 RPM on the machine.
20mm Gun Drill in Mild Steel
Cutting speed: 80 m/min
RPM = (80 x 1000) / (3.14 x 20) = 80,000 / 62.8 = 1274 RPM
I round to 1275 RPM.
Same Diameters in Aluminum
Aluminum wants much higher cutting speeds. I use 200 m/min as my starting point.
- 6mm: (200 x 1000) / (3.14 x 6) = 10,615 RPM – set to 10,600 RPM
- 10mm: (200 x 1000) / (3.14 x 10) = 6369 RPM – set to 6350 RPM
- 20mm: (200 x 1000) / (3.14 x 20) = 3185 RPM – set to 3200 RPM
Notice how the RPM drops as the diameter increases. This is the inverse relationship at the heart of the formula: double the diameter, halve the speed.
How to Adjust for Deep Holes vs Shallow Holes
The formula gives you a starting point. The depth of the hole changes everything.
I use the length-to-diameter (L/D) ratio to decide how much to reduce speed:
| L/D Ratio | Speed Reduction |
|---|---|
| Up to 10:1 | No reduction |
| 10:1 to 20:1 | Reduce 10-20% |
| 20:1 to 50:1 | Reduce 20-35% |
| 50:1 to 100:1 | Reduce 35-50% |
| Over 100:1 | Reduce 50% or more, consult manufacturer |
The logic is simple: deeper holes mean more friction, worse chip evacuation, and higher heat buildup at the tool tip. Running at full calculated RPM in a 50:1 hole will overheat the drill in minutes. I start conservative and work up if the chips look good.
For a 10mm drill going 500mm deep (50:1 L/D), I take my 2547 RPM calculation and reduce it by roughly 40%, landing around 1500 RPM for the first pass.
How to Calculate Penetration Rate from RPM and Feed
Spindle speed is only half the picture. Penetration rate (how fast the drill advances through the material) depends on both RPM and feed per revolution.
Penetration Rate (mm/min) = RPM x Feed per Revolution (mm/rev)
Most gun drill manufacturers recommend a feed between 0.01 and 0.05 mm/rev, depending on diameter and material. I use 0.02 mm/rev as my baseline for steel and 0.04 mm/rev for aluminum.
Here is what that works out to for common diameters:
| Diameter | Material | RPM | Feed (mm/rev) | Penetration Rate (mm/min) |
|---|---|---|---|---|
| 6mm | Mild Steel | 4200 | 0.015 | 63 |
| 6mm | Aluminum | 10,600 | 0.04 | 424 |
| 10mm | Mild Steel | 2550 | 0.02 | 51 |
| 10mm | Aluminum | 6350 | 0.04 | 254 |
| 20mm | Mild Steel | 1275 | 0.025 | 31.9 |
| 20mm | Aluminum | 3200 | 0.05 | 160 |
| 30mm | Mild Steel | 850 | 0.03 | 25.5 |
| 30mm | Aluminum | 2120 | 0.05 | 106 |
These are starting values. I adjust feed based on chip formation – thin chips mean I can increase feed, while segmented or broken chips tell me to back off.
RPM Quick Reference Table
I keep this table laminated and tacked to the wall next to my machine. It covers the diameters and materials I see most often:
| Diameter | Mild Steel (80 m/min) | Alloy Steel (60 m/min) | Stainless (40 m/min) | Aluminum (200 m/min) |
|---|---|---|---|---|
| 5mm | 5096 RPM | 3822 RPM | 2548 RPM | 12,739 RPM |
| 6mm | 4246 RPM | 3185 RPM | 2123 RPM | 10,615 RPM |
| 10mm | 2548 RPM | 1911 RPM | 1274 RPM | 6369 RPM |
| 20mm | 1274 RPM | 956 RPM | 637 RPM | 3185 RPM |
| 30mm | 849 RPM | 637 RPM | 425 RPM | 2123 RPM |
| 50mm | 510 RPM | 382 RPM | 255 RPM | 1274 RPM |
The pattern is consistent: every diameter step changes RPM by the ratio of the diameters. Once you know one row, you can derive the rest.
Common Mistakes
I have made every mistake on this list at least once.
Running too slow for the diameter. Large-diameter drills at low RPM seem safe, but running too far below the calculated speed encourages rubbing instead of cutting. The tool dulls faster and surface finish suffers. Stay within 20% of the calculated value unless L/D reduction forces you lower.
Not accounting for tool wear. A fresh gun drill can handle higher speeds. As the tool wears, the cutting edge dulls and generates more heat. I drop RPM by 10-15% after the first regrind, and another 10% after the second. Track your regrinds and adjust accordingly.
Using the same RPM for shallow and deep holes. As covered above, depth changes everything. A 10:1 hole and a 50:1 hole in the same material should not run at the same speed. Always factor in L/D.
Ignoring coolant pressure and flow. Gun drilling relies on high-pressure coolant to clear chips. If your coolant pressure drops below 30 bar (435 PSI) at the tool tip, reduce RPM by 20% until you sort out the coolant issue. Running full speed with inadequate coolant guarantees a crash.
Rounding the wrong way. Always round down, not up. 2548 RPM rounded to 2600 pushes the tool harder than recommended. I round to the nearest 25 or 50 RPM below the calculated value.
Related Guides
I cover the broader parameter selection process in the Deep Hole Drilling Parameters Guide. For a full table of speeds and feeds across more materials and tool types, see the Gun Drilling Speeds and Feeds Reference.
Key Takeaways
- RPM follows a simple inverse relationship with diameter. Learn the formula and you can calculate any job in seconds.
- Always adjust for L/D ratio before locking in your speed. Deep holes demand conservative RPM.
- Penetration rate depends on both RPM and feed. Calculate it to estimate cycle time and spot feed problems early.
- Round RPM values down, not up, and adjust for tool wear across the life of the drill.
- Use the quick reference table for everyday materials and diameters, but recalculate whenever you change material or tool size.