How to Do Deep Engraving Stainless Steel by CNC Machine
Deep engraving stainless steel is not a light marking pass. It is a controlled milling operation in a material that work-hardens under the cutter. This guide is for engineers and buyers who need 0.3 mm to 2 mm deep lettering, logos, or cavities that stay sharp across a full production run. Read it to pick the right tool, set conservative parameters, and decide when a 3-axis setup is enough and when you need 5-axis.
In this article
- 1
- 2
- 3
- 4
- 5
- 6
- 7
Key takeaways
Why Deep Engraving Stainless Steel by CNC Machine Fights Back
Stainless steel resists corrosion because of chromium, and that same alloying makes it stubborn to cut. Grades like 304, 316L, and 17-4PH combine high tensile strength with low thermal conductivity. Heat from the cut has nowhere to go, so it piles up at the tool edge while the workpiece stays cool. That heat is what dulls cutters and pushes the surface into a hardened state.
Work-hardening is the main trap. Every time the cutting edge rubs instead of shears, the surface layer gets harder. A light spring pass with a dull tool does more damage than a firm, correct cut. Operators who try to sneak up on depth with many tiny passes often end up with the worst tool wear of all.
A second factor is chip evacuation in narrow grooves. Deep engraving produces small chips that pack into the slot and get recut. Recutting multiplies heat and ruins the floor finish. Air blast or through-spindle coolant solves most of this, but the toolpath has to give chips a way out.
This is why deep engraving should be planned as a milling operation from the start: defined tool, defined depth of cut, defined pass count. Treating it as a decoration step at the end of the process is how parts get scrapped late.
- 1Low thermal conductivityHeat stays at the cutting edge instead of spreading into the part.
- 2Work-hardeningRubbing hardens the surface and accelerates the next tool's wear.
- 3Chip packingNarrow slots recut chips unless coolant or air clears them.
Choosing Tool Geometry for Engraving Stainless Steel by CNC Machine
For shallow detail under 0.2 mm deep, a 60° or 90° included-angle carbide engraving cutter is fine. Its point gives crisp corners and small text. Once the depth target goes past 0.2 mm, the point becomes a problem. The tip has almost no cutting speed, so it rubs, hardens the floor, and snaps. Depth targets of 0.3 mm or more call for a micro end mill.
Pick a two-flute or three-flute micro end mill with a corner radius. A 0.5 mm radius on a 2 mm cutter spreads load and survives the hard floor layer. AlTiN or TiAlN coating helps at higher surface speeds; uncoated carbide works at lower speeds if the coolant is clean. Avoid long flute lengths. A short, stiff cutter deflects less at the same depth.
Corner radius matters more than most people expect. A sharp-cornered micro end mill concentrates stress exactly where the hardened layer sits. A small radius, often 0.1 mm to 0.5 mm, can triple tool life in 316L without visibly changing the engraved corner in most logo work.
Keep a separate finishing cutter. One tool doing roughing and finishing will wear its edge before the run ends, and depth will drift. Two tools cost more per part in tooling, but they hold depth and reduce scrap. On medical and aerospace parts, that trade is easy to justify.
- 1V-bits for shallow60° or 90° point cutters suit detail under 0.2 mm deep.
- 2Micro end mills for depthUse 2–3 flute carbide with a 0.1–0.5 mm corner radius.
- 3Short flute lengthLess deflection, better depth control in hardened surfaces.
Speeds, Feeds, and Stepover Ranges That Work
Start conservatively and tune from the first part. For a 2 mm coated carbide end mill in 304 stainless, a surface speed around 60 to 90 m/min gives reasonable tool life on a rigid setup. In 316L, drop to 45 to 70 m/min because the molybdenum content raises cutting resistance. For 17-4PH in the H900 condition, stay near the low end and expect shorter tool life.
Feed per tooth should be high enough to shear rather than rub. A range of 0.01 to 0.03 mm per tooth works for micro end mills in stainless. Many shops set feeds too low for fear of breaking small tools, then wonder why the edge wears out in minutes. Rubbing is the enemy, not a firm chip load.
Radial stepover for finishing stays between 8% and 12% of cutter diameter. Axial depth of cut per pass for a 2 mm cutter sits around 0.1 to 0.3 mm. If the target depth is 1 mm, that means several passes. Trying to remove 1 mm in one axial bite overloads a micro tool and snaps it.
Coolant choice is not cosmetic. Flood coolant with good pressure flushes chips from narrow grooves. Through-spindle coolant is better for deep, narrow features. Air blast alone works on open lettering but fails in slots where chips pack. Whatever you choose, aim the stream at the cut, not at the part surface.
- 1Surface speed60–90 m/min in 304; 45–70 m/min in 316L.
- 2Feed per tooth0.01–0.03 mm. Too low rubs and hardens the floor.
- 3Stepover8–12% of cutter diameter for finishing passes.
- 4Axial depth0.1–0.3 mm per pass on a 2 mm cutter.
Holding Depth Tolerance on a Production Run
Depth tolerance is where most runs fail, not corner sharpness. Tool wear changes effective length, so a program that cuts 0.50 mm on part one may cut 0.44 mm on part 200. The fix is a documented offset schedule. Measure the first part, then measure again at fixed intervals and log the offset change.
Heat is the other drift source. If the spindle and fixture warm up during the first hour, depth shifts with thermal growth. Run a warm-up cycle before the production batch, and keep the coolant temperature stable. On tight jobs, measure the first part after the machine has been running for a while, not from a cold start.
For depths above 0.5 mm, plan at least two passes. A single deep pass in stainless loads the cutter heavily and leaves a poor floor. Two passes, one roughing and one finishing, also give you a chance to correct depth before the final cut. This is basic, and it is the single most reliable habit for holding ±0.005 mm on engraved features.
Record the parameters that worked. Material grade, tool part number, surface speed, stepover, pass count, and offset drift per 100 parts. That record is what makes the second run cheaper than the first.
- 1Offset scheduleLog tool offset change every 20–50 parts and act on it.
- 2Thermal warm-upRun the spindle before the batch so depth does not drift.
- 3Two-pass minimumRough then finish for any depth above 0.5 mm.
Step by Step Deep Engraving Setup
- 11. Fix the workpiece rigidlyVibration kills micro tools. Clamp close to the engraving area or use a fixture plate. Avoid long overhangs on the part and on the tool holder. A 2 mm cutter sticking 30 mm out of the collet will chatter before it cuts.
- 22. Set zero on the actual surfaceTouch off on the material surface, not on the fixture. Stainless plate thickness varies, and engraving depth is measured from the top face. Program depth as a positive value below Z0 so the toolpath stays readable.
- 33. Rough the cavityUse a slightly smaller end mill or a relieved cutter to remove most of the depth. Leave 0.05 to 0.1 mm of stock on the floor and walls. Keep axial depth at 0.1 to 0.3 mm per pass.
- 44. Finish with a dedicated toolSwitch to a fresh micro end mill with the corner radius you specified. Run 8 to 12% stepover and a light axial cut. This pass sets the final depth and the wall finish.
- 55. Clear chips continuouslyFlood coolant or through-spindle coolant from the first cut. If you see chips sitting in the groove, stop and fix the coolant aim. Recut chips are the fastest route to a scrapped depth.
- 66. Measure depth on the machineUse a depth gauge or a dial indicator on the first part. Check the deepest and shallowest letters. If depth is short, adjust the offset, not the program, so you keep a record of tool wear.
- 77. Monitor wear and re-zeroRecord the offset change after every 20 to 50 parts, depending on depth. When the offset shift passes your tolerance band, change the tool. Do not run a second batch on a worn cutter.
When 3-Axis Is Enough and When You Need 5-Axis
Match the machine to the feature geometry, not to habit.
| Feature | 3-axis setup | 5-axis setup |
|---|---|---|
| Flat plate, engraving on top face | Enough | Not needed |
| Cylindrical or tapered surface | Rotary table helps | Better option |
| Side wall of a deep pocket | Limited reach | Tilt keeps engagement stable |
| 0.5 mm deep logo on a curved implant | Risk of chatter | Preferred for tool life |
| Long, narrow slots | Tool deflection grows | Tilt reduces deflection |
| One-off prototype, flat lettering | Fastest to set up | Overkill |
Plan the depth, not just the picture
Deep engraving stainless steel succeeds when you treat it as a milling operation with a defined tool, pass count, and offset schedule. If your feature is under 0.2 mm deep and flat, a 3-axis machine with a V-bit is enough. If it goes deeper or sits on a curved surface, use a micro end mill and consider 5-axis so the cutter stays engaged.
Common Questions
How deep can you engrave stainless steel with a CNC machine?
Depth is limited by tool diameter and rigidity, not by a fixed ceiling. A 2 mm micro end mill can reach 1 to 2 mm deep with multiple passes. Deeper features need a larger cutter or a different process such as EDM.
For most logos and lettering, 0.3 to 0.8 mm deep is the practical range. It reads clearly, holds up to wear, and keeps tool life predictable.
Should I use a V-bit or an end mill for deep engraving?
Use a V-bit for detail under 0.2 mm deep. Its point gives sharp corners and fine text.
Switch to a micro end mill with a corner radius once depth passes 0.2 mm. The V-bit tip has almost no cutting speed and will rub, harden the floor, and break.
Why does my engraving depth come out shallow?
Tool wear is the usual cause. The cutter gets shorter as the edge wears, so the same program cuts less depth over time.
Check coolant aim and chip evacuation too. Packed chips lift the effective cutting point and leave a rough, shallow floor. Adjust the tool offset before changing the program.
What coolant works best for engraving stainless steel?
Flood coolant at good pressure handles most work. Through-spindle coolant is better for narrow, deep grooves where chips pack.
Air blast works only on open lettering with a clear chip path. If chips sit in the cut, change the coolant method before touching speeds and feeds.
How do you keep the walls straight in a deep engraved slot?
Keep radial stepover low, between 8% and 12% of cutter diameter, and use a short, stiff cutter. Climb milling also helps, because it keeps the load even on the finishing pass.
If walls still taper, the tool is deflecting. Reduce axial depth per pass or move the job to a 5-axis setup so the cutter can tilt and stay engaged.
Can you deep engrave 316L and 17-4PH the same way as 304?
No. 316L resists cutting more than 304 because of its molybdenum content, so drop surface speed to 45 to 70 m/min. 17-4PH in the H900 condition is harder again and wears tools faster.
Plan shorter tool-change intervals and more frequent depth checks on these grades. The geometry strategy stays the same, but the wear rate does not.
Send us your engraving drawing
Upload your file and we will review depth, tool access, and pass count, then quote within 12 hours. DFM feedback comes with the quote at no cost.
12-hour quoteNo minimum order quantityNDA on request
More from the shop floor
We publish setup notes, tooling trials and inspection data from the factory floor.
