Feed and speed optimization is the most effective way I have found to reduce cost per hole in deep hole drilling. The right parameters balance material removal rate against tool life, and the sweet spot can double or triple the number of good holes per drill. A systematic approach beats guesswork every time.
Starting Point: Manufacturer Recommendations
I start every new material or tool with the manufacturer recommended parameters. Tool manufacturers have tested their drills across a range of conditions and their starting point is reliable for getting the first part through safely.
For a typical carbide gun drill in medium-carbon steel (1045, 20-30 HRC):
| Drill Diameter | Recommended Speed (SFM) | Recommended Feed (mm/rev) |
|---|---|---|
| 5 mm | 150-200 (2,400-3,200 RPM) | 0.015-0.025 |
| 10 mm | 130-170 (1,300-1,700 RPM) | 0.020-0.035 |
| 15 mm | 120-150 (800-1,000 RPM) | 0.030-0.045 |
| 20 mm | 110-140 (550-700 RPM) | 0.035-0.050 |
| 30 mm (BTA) | 90-120 (300-400 RPM) | 0.050-0.080 |
I take the middle of the recommended range as my starting point. For a 10 mm drill in 1045 steel, that is 1,500 RPM and 0.028 mm/rev.
Feed Optimization First, Speed Second
Feed and speed do not affect tool life equally. My optimization sequence is to dial in the feed first because changing the feed affects chip formation more directly. Once the feed produces good chips, I adjust the speed to hit the tool life target.
My feed optimization process:
- Run a test at the manufacturer feed and record tool life in millimeters drilled.
- Increase feed by 10 percent and run another test.
- If tool life stays the same or improves, increase feed by another 10 percent.
- Repeat until tool life decreases by more than 10 percent.
- Step back to the previous feed value where tool life was best.
In my experience, the feed that gives the best tool life is usually 10-30 percent higher than the manufacturer starting point. The increased feed creates thicker chips that carry more heat away from the cutting edge.
Speed Effect on Tool Life
The speed has a much larger effect on tool life than the feed. This relationship is captured in the Taylor tool life equation, and in my real-world measurements it holds true:
| Speed Change | Typical Effect on Tool Life |
|---|---|
| Increase by 10 percent | Decrease by 30-50 percent |
| Increase by 20 percent | Decrease by 60-75 percent |
| Decrease by 10 percent | Increase by 50-100 percent |
| Decrease by 20 percent | Increase by 100-200 percent |
I find the speed that gives acceptable tool life at the optimized feed. The target tool life depends on the production volume:
| Production Volume | Target Tool Life (mm drilled) | Strategy |
|---|---|---|
| Under 100 parts/year | 5,000-10,000 mm | Run faster, accept shorter tool life |
| 100-1,000 parts/year | 15,000-25,000 mm | Balance speed and tool life |
| Over 1,000 parts/year | 25,000-50,000 mm | Run slower, maximize tool life |
For high-volume production, reducing the speed by 15 percent can increase tool life by 100 percent. The cycle time increase is only 15 percent but the tool cost per hole is cut in half. The math favors lower speeds for volume production.
Chip Shape as a Diagnostic Tool
The chip shape tells me whether the parameters are correct without measuring anything. I collect chips from every test cut and examine them.
| Chip Shape | What It Means | Action |
|---|---|---|
| Short, broken “C” or “6” shapes | Good chip control | Keep parameters |
| Long, stringy ribbons | Feed too low or material too soft | Increase feed |
| Fine powder or dust | Speed too high or feed too low | Reduce speed, increase feed |
| Blue or discolored chips | Excessive heat, speed too high | Reduce speed |
| Chips that pack in the flute | Feed too high for chip evacuation | Reduce feed |
Short, broken chips indicate good parameters. Long stringy chips or fine powder mean the parameters need adjustment. I have dialed in parameters for a new material in three test cuts just by watching the chip shape.
Documenting Optimized Parameters
Every optimized parameter set goes into a spreadsheet organized by material, hardness, drill diameter, and drill type. The documentation saves setup time on repeat jobs and builds a knowledge base that makes new material optimization faster.
My parameter record includes:
- Material type and hardness
- Drill diameter and type (gun drill, BTA head, ejector)
- Cutting speed in SFM and RPM
- Feed rate in mm/rev and mm/min
- Coolant pressure and type
- Tool life in millimeters drilled
- Surface finish achieved (Ra)
- Chip shape observations
Over time, the documented parameters let me predict the starting point for a new material within 10-15 percent of the optimal settings. The first test cut is close to the final value.
Key Takeaways
Feed and speed optimization is a simple process that delivers measurable results. I optimize feed first for chip control, then adjust speed for tool life. The chip shape tells me instantly whether the parameters are in the right range. The speed has a disproportionate effect on tool life, so for production work I err on the side of slower speeds. Documenting every optimized parameter set turns one-time experiments into reusable knowledge that speeds up every future job.