Machinability Ratings Explained

The AISI 1212 Baseline System

The American Iron and Steel Institute (AISI) established AISI 1212 free-machining steel as the 100% machinability baseline. All other materials are rated relative to this benchmark. A material rated at 50% means cutting tools last approximately half as long (at the same cutting speed) as they do on 1212. A material rated at 150% means tools last 50% longer.

The original tests measured tool life at a fixed surface speed using a specific tool geometry, cutting fluid, and depth of cut. The cutting speed that produced 60 minutes of tool life on 1212 was the reference point. Other materials were tested at the same speed, and the tool life ratio became the machinability rating.

An alternative interpretation: the machinability rating represents the percentage of the baseline cutting speed you can use and achieve comparable tool life. A 60% material should be run at roughly 60% of the speed that works for 1212 to get similar tool life. This is how most machinists use the ratings in practice.

What Makes a Material Easy or Hard to Machine

Hardness: Harder materials require more cutting force and generate more heat. But hardness alone does not determine machinability — some hard materials (like leaded brass at 80+ HRB) machine easily because the chips break cleanly and the cutting forces are low despite the hardness.

Ductility: Highly ductile materials (like pure copper, annealed stainless, and low-carbon steel) form long, stringy chips that wrap around the tool, clog flutes, and produce poor surface finish. The chip does not want to break, which makes chip control the primary challenge. Adding sulfur, lead, or other chip-breaking elements solves this problem — that is why 303 stainless machines so much better than 304.

Work Hardening: Materials that work-harden during cutting (austenitic stainless steels, nickel alloys, titanium) present a unique challenge. If the tool dwells, rubs, or takes a light cut, it hardens the surface layer, making the next pass more difficult. The solution is to always maintain positive chip load — keep the tool cutting, never rubbing.

Abrasiveness: Materials with hard inclusions (cast iron with sand, aluminum with high silicon, some stainless castings) wear cutting edges rapidly through abrasion rather than heat or adhesion. This shortens tool life even when cutting forces and temperatures are moderate. Use ceramic or CBN inserts for highly abrasive materials.

Thermal conductivity: Materials with poor thermal conductivity (titanium, Inconel) concentrate heat at the cutting edge because the workpiece does not conduct heat away from the cutting zone. This accelerates tool wear and limits practical cutting speeds.

Why Different Sources Give Different Ratings

If you look up the machinability of 4140 steel in three different references, you might find values of 55%, 65%, and 50%. This is not because the references are wrong — it is because machinability is not a fixed property of the material. It depends on the test conditions, and different sources test differently.

Variables that change the rating: tool material (HSS vs carbide), tool geometry (positive vs negative rake), cutting speed, depth of cut, feed rate, cutting fluid type and delivery method, and the criterion used to define end of tool life (flank wear, crater wear, surface finish degradation, or total failure). A carbide insert test and an HSS tool life test on the same material can produce ratings 20 percentage points apart.

The practical takeaway: treat machinability ratings as approximate guides, not precise specifications. A material rated at 55% in one source and 65% in another is in the same general category — harder than free-machining steel, easier than stainless. Use the rating to set a starting point for speeds and feeds, then adjust based on actual cutting performance in your shop with your tooling.

Translating Ratings into Speeds and Feeds

The most practical use of machinability ratings is scaling cutting parameters from a known material to an unknown one. If you have proven speeds and feeds for 1045 steel (machinability ~55%) and need to machine 316 stainless (machinability ~36%), scale the surface speed proportionally: New SFM = Old SFM × (36/55) = about 65% of your 1045 speed.

Feed rate scaling is less proportional. Lower machinability materials generally benefit from maintaining or even increasing the feed per tooth to keep the chip thick enough to break cleanly and prevent work hardening. Reduce speed (SFM) first, not feed. A slower speed with a substantial chip load produces better results than a fast speed with a light chip on difficult materials.

The SFM ranges published in tooling catalogs and this tool's material database are a more direct way to set starting parameters than scaling from ratings. But when you encounter a material not in your catalog, the rating-based scaling method gets you in the right neighborhood quickly.