GGG50 / EN-GJS-500-7 ductile iron: cutting speed and feed

Optimize your machining processes with our online cutting parameters calculator. Select the operation type (turning, milling, drilling or threading) and instantly get the critical calculations for your shop: cutting speed (Vc), revolutions per minute (RPM), feed per revolution or per tooth, machining time and the theoretical roughness (Ra / Rz) based on the insert nose radius. To fine-tune those values live at the machine, use the interactive machining calculator.

Cutting calculator

Step 1

Which operation are you machining?

Do you want to adjust these values live?

Here you get the recommendation (Vc, feed, roughness, threading). In the interactive machining calculator you can move Vc, diameter, RPM and feed with linked scales, locks and time/power estimation.

Open interactive calculator →

GGG50 ductile iron turns and mills at 130-220 m/min (about 425-720 SFM) with 0.28 mm/rev or 0.11 mm per tooth, drills at 91-165 m/min with 0.2 mm/rev and taps at 46-99 m/min. It runs slower than grey iron because spheroidal graphite makes it far tougher. In practice it behaves like a hybrid between cast iron and steel, and it needs to be treated as one.

EN-GJS-500-7 · DIN GGG50 · 200 HB · ISO group K

Recommended speeds and feeds

Operation	Vc (m/min)	Feed	Shop note
Turning	130–220	0.28 mm/rev	130-220 m/min at 0.28 mm/rev. Unlike grey iron, here you do need a chipbreaker: ductile iron chips can come off in long strings that wrap the turret, especially in ferritic grades and at low feeds.
Milling	130–220	0.11 mm/tooth	130-220 m/min with 0.11 mm per tooth, preferably dry or with air so you do not thermally crack the edge. ISO K inserts with a heat-resistant coating outlast a steel geometry when roughing blocks.
Drilling	91–165	0.2 mm/rev	91-165 m/min at 0.2 mm/rev. Ductile iron does not break out on exit like grey iron, but the chip is longer and has to be cleared: through-coolant or programmed pecks every three or four diameters of depth.
Threading	46–99	0.2 mm/rev	46-99 m/min with a cut tap. Ferritic grades will take careful form tapping thanks to their extra ductility, but pearlitic grades crack the thread; if the thread carries load, cut tap or thread mill.

Starting values for coated carbide in medium cutting. Fine-tune them in the calculator for your tool, type of pass and safety margin.

How it behaves when cutting

In GGG50 the graphite sits as spheres rather than flakes, so it no longer acts as a fracture plane: the material gains ductility and tensile strength (hence the 500 MPa in its designation) and loses the clean fracture that makes grey iron so easy. The chip comes off in longer pieces with some tendency to stick, and more heat is generated. At around 200 HB average, the matrix can be ferritic, pearlitic or mixed, and that proportion changes the result noticeably: pearlitic areas are harder and more abrasive. In big castings with uneven cooling you can also hit extremely hard localised carbides.

Ductile against grey: what actually changes

Going from flake to spheroidal graphite turns a brittle, abrasive material into a tough, ductile one. Three things follow on the shop floor. First, you have to drop speed from 150-250 to 130-220 m/min because more heat is generated and wear accelerates. Second, chip control becomes a real job, with chipbreakers and adequate feeds, where grey iron needed neither. Third, edge break-out almost disappears, so tool exits stop being a problem. Anyone who programs ductile iron with grey iron parameters notices the insert wear before anything else.

Ferritic or pearlitic matrix: hardness is not uniform

A GGG50 is by definition a mix of ferrite and pearlite, and the ratio varies between heats and even between areas of the same casting depending on section thickness and cooling rate. Ferrite is soft and sticky, pearlite is harder and abrasive, and a large part can be 170 HB in the middle and 240 HB in a thin rib. If tool wear swings a lot between parts in the same batch, suspect the material before you blame the program. Running mid-range, around 170-180 m/min, gives the most consistent life when the casting is not homogeneous.

Hard carbides in chilled areas

In corners, abrupt section changes and casting edges, rapid cooling can form extremely hard iron carbides - localised white iron. That zone does not cut: it destroys the edge the instant it touches it. You spot it by a characteristic squeal and by sudden wear at one specific point in the program. If the defect repeats in the same area part after part, it is the casting and not the tooling, and the fix is annealing the raw castings or a conversation with the foundry. In the meantime, reduce speed and reinforce the edge for that stretch of the program.

Quick shop tips

Do not reuse the grey iron program: drop to 130-220 m/min and add a chipbreaker.
If wear varies a lot from part to part, check hardness; the ferrite-to-pearlite ratio changes between heats.
Mill dry or with air, just like grey iron, to avoid thermal cracking on the edge.
A squeal plus sudden wear always at the same point in the program points to hard chill carbides.
In drilling, program pecks every three or four diameters: ductile iron chips are longer than you expect.
For threads that carry load, use a cut tap or a thread mill; form tapping only really works in ferritic grades.

Frequently Asked Questions (FAQ)

What is the difference between machining GG25 and GGG50?

Ductile iron is tougher and more ductile: it wants less speed (130-220 against 150-250 m/min), makes a longer chip that has to be broken, and wears tools more through heat. In return, it does not chip out exit edges the way grey iron does.

Does ductile iron need coolant?

In continuous turning it can help control temperature and dust, but in milling dry or air is still better, because intermittent flood cracks the edge. In deep drilling, through-coolant is worth having to clear the chip.

What Vc do I use on GGG50 with HSS tooling?

Around 45-75 m/min, a third of the carbide range. In hard pearlitic areas HSS wears very quickly, so for production runs coated ISO K carbide works out far cheaper.

Why does my insert always break at the same point on the part?

Almost certainly hard chill carbides in that area, typical of corners and section changes. It is not a parameter problem: reduce speed over that stretch and raise annealing of the raw castings with the foundry.

Can GGG50 be form tapped?

Only in ferritic-matrix grades and with care, because ductility is limited. In pearlitic grades the thread comes out cracked and you need a cut tap or a thread mill.

Similar materials

GG25 / EN-GJL-250 grey cast iron: cutting speed and feed

Cutting speed and feed for GG25 / EN-GJL-250 grey cast iron: why it is machined dry, how to survive the casting skin and how to stop edges chipping out.

42CrMo4 / 4140 alloy steel: cutting speed and feed rate

How to machine 42CrMo4 / 4140 quenched and tempered: cutting speed and feed per operation, coatings that survive and Vc matched to the bar's real hardness.

C45 / 1045 steel: cutting speed and feed rate

Speeds and feeds for C45 / AISI 1045 steel: Vc and feed per operation, and how much changes when the bar arrives quenched and tempered, not normalised.

Related tools

RPM, feeds and machining time calculator

Calculate cutting speed, RPM, feeds and pass time for milling, turning and drilling. Adjust values with linked scales and look up starting values by material.

Calculate cycle time

Estimate CNC turning and milling cycle time from G-code. Calculate parts per hour with a breakdown of cutting, rapids, canned cycles and tool changes.

Machining quote

Instant machining quote: material, machine time, setup per batch, secondary operations and margin. Free, no sign-up.