Drilling — modes

How to use the drilling mode calculator

Specify drill diameter, ISO material, tool type (HSS/HSS-Co/Carbide/Insert), coolant, hole type and depth. The calculator works in two modes: “Vc → RPM” (set the cutting speed - get the speed) and “RPM → Vc” (set the speed - get the speed). If Vc or feed is not specified, the calculator will substitute starting values ​​from the table. Result: RPM, table feed Vf, MRR, recommended peck and cycle type (G73 / G83), with risk level assessment. The visual L/D scale shows depth relative to thresholds.

Why drilling modes cannot be copied from the catalog without correction

Catalog values ​​of Vc and f are given for ideal conditions: rigid clamp, new tool, through-tool coolant, medium depth through hole. On a real machine, the conditions are almost always worse: the coolant is external, the hole is blind, the depth is 8×D, the material is riveted. The calculator adjusts the starting values ​​for each of these factors - and shows how your situation differs from the ideal.

What affects the modes

Workpiece material (ISO).Determines the Vc and feed range. Aluminum (N) allows a Vc of 150–300 m/min for carbide. Steel (P) - 60–120. Stainless steel (M) - 40–80. Heat resistant (S) - only 20–45. Hardened (H) - 25–55. Each group also requires a feed adjustment: stainless steel - minus 22% of the base, heat-resistant - minus 35%.

Tool type. An HSS drill operates at speeds 3–5 times lower than a carbide drill, and with a feed rate half as much. HSS-Co (cobalt) is an intermediate option. Flap drills allow high Vc, but are more sensitive to runout and rigidity. The calculator takes into account the type of tool in both formulas - both for speed and feed.

Cooling.Through-tool (through the tool) - standard for deep drilling. Flood (external) - works up to L/D ≈ 5. MQL - limited, flow is reduced by 10%. Dry drilling - feed rate is reduced by 20%, increased risk of overheating. The calculator takes into account the type of cooling in both supply, peck rating, and risk level.

Depth (L/D). When L/D < 5 - standard conditions. At 5–8 - feed is reduced by 15%, peck is desirable. At 8–12 - feed minus 30% of the base, peck is required. When > 12 - special strategy: gun drill, HPC, or step drilling. The calculator shows L/D on a visual scale and automatically adjusts all parameters.

Drilling cycle.G73 (chip-break) - short retraction of 0.5–1.0 mm to break chips. Faster, but only suitable with good offset. G83 (full retract) - full withdrawal of the drill for chip evacuation. Slower, but more reliable for blind holes and depths > 8×D. The calculator recommends a cycle based on a combination of factors: depth, material, coolant, type of hole.

Frequently Asked Questions

How does the calculator calculate the feed? The base is a table of feeds by diameter for carbide (industry standard). Then the following multipliers are applied sequentially: tool type (HSS = ×0.55, HSS-Co = ×0.65), material (stainless steel = ×0.78, heat resistant = ×0.65), cooling (dry = ×0.80), depth (L/D ≥ 8 = ×0.85), hole type (blind = ×0.92), priority (safety = ×0.90). The final range is [lo, hi], the middle point is the starting value.

When is G83 needed instead of G73? The calculator uses scoring: blind hole (+3), L/D ≥ 8 (+3), L/D ≥ 12 (+4), stainless steel (+2), heat resistant (+3), dry (+2). If the amount is ≥ 6, G83 is recommended. Practically: a blind hole in stainless steel deeper than 5×D is almost always G83.

What is Peck Q and how to choose it? Peck Q is the depth of one “bite” of the drill before retraction. The calculator calculates Q as a fraction of the diameter (0.5–0.8×D), adjusted for material, cooling and depth. For HSS in stainless steel at L/D = 10 - Q can be only 0.3×D. For carbide with through-tool in steel - up to 0.8×D.

Why is MRR calculated differently when drilling than when milling? Because the drill removes a full cylinder: MRR = (π×D²/4) × Vf / 1000. The cross-sectional area is a full circle, not a stripe ae×ap as in milling. Therefore, the MRR for drilling is usually higher than for milling the same diameter.

Is it possible to drill hardened steel (H) with a regular drill? HSS - no, it breaks or burns. HSS-Co - only at HRC ≤ 48 and shallow depths. Carbide alloy - yes, at Vc 25–55 m/min, reduced feed (×0.60 from the base) and stable coolant. Flat drills with CBN inserts - for serial machining. The calculator automatically reduces all parameters for group H.

Need help selecting a drill, modes or strategy for deep drilling? Contact our specialists - we will select the tools and parameters for your material and machine.