We use technical and security cookies and, only if you accept, analytics with no cross-site tracking. More in the Cookie policy and Privacy policy.
We use first-party cookies and technical storage to make the site work, Google reCAPTCHA security technology and, only if you accept, Vercel analytics (no cookies, no cross-site tracking). You can accept or reject analytics; both options are equivalent and you can change your choice at any time. More info: Cookie policy, Privacy policy, Legal notice and Terms and conditions.
GG25 / EN-GJL-250 grey cast 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.
GG25 grey cast iron turns and mills at 150-250 m/min (about 490-820 SFM) with 0.3 mm/rev or 0.12 mm per tooth, drills at 105-188 m/min with 0.22 mm/rev and taps at 53-113 m/min. It is one of the most forgiving materials on the floor: the chip breaks itself and the cut is stable. Its two problems are not at the cutting edge - they are the abrasive dust it makes and the edges it chips out on exit.
EN-GJL-250 · DIN GG25 · 220 HB · ISO group K
Recommended speeds and feeds
Operation
Vc (m/min)
Feed
Shop note
Turning
150–250
0.3 mm/rev
150-250 m/min at 0.3 mm/rev, dry, with a coated carbide insert; for long runs in continuous cutting, ceramic or silicon nitride will go far faster, but at that point coolant stops being optional and becomes forbidden.
Milling
150–250
0.12 mm/tooth
150-250 m/min with 0.12 mm per tooth. Coolant here is counterproductive: the edge is entering and leaving the cut, and the hot-cold shock cracks the insert in a comb pattern. Run dry and pull the dust away with air or extraction.
Drilling
105–188
0.22 mm/rev
105-188 m/min at 0.22 mm/rev. GG25 drills beautifully, but the drill breaks out the far edge on exit: halve the feed for the last millimetre or put a chamfer on the breakout face.
Threading
53–113
0.22 mm/rev
53-113 m/min and always with a cut tap: cast iron does not flow, so a form tap cannot roll the thread and only manages to crack it. Straight flutes are fine, because the dusty chip falls out under gravity.
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
The flake graphite that gives GG25 its colour and its vibration damping also acts as a built-in fracture plane: the chip never forms a continuous ribbon, it fractures into flakes and dust. That means moderate cutting forces, no tendency to weld onto the tool and perfect chip control with no chipbreaker at all. In exchange, that dust is abrasive, works its way into ways and wipers, and the as-cast skin brings sand and oxide that destroy an edge on the first pass. At 220 HB, GG25 is also weak in tension, so the edge where the tool exits will break away unless you protect it.
Casting skin: the pass that kills inserts
A fresh casting carries an outer layer of moulding sand residue, oxide and sometimes chilled zones full of extremely hard carbides. That skin can wear out a new insert in a single pass if you enter at catalogue speed. Take 30% off the speed for the first pass, go deep enough to get underneath the layer (2 mm or more) and use a reinforced edge with a land. Once the skin is gone, the material underneath is homogeneous, and that is where you can push up to 200-250 m/min and get the full tool life the catalogue promises.
Dry or flood: why it is nearly always dry
Grey iron is traditionally machined dry for two reasons. The first is that dust mixed with coolant makes a black slurry that sticks to everything, blocks filters and fouls the whole machine. The second, more technical, is that in interrupted cuts such as milling, intermittent flood puts the edge through heating and cooling cycles that produce transverse thermal cracks - the comb pattern - until the insert crumbles. If you need to control the dust, use extraction or compressed air. Only deep drilling or very tight dimensional work justifies coolant.
Edge chipping: the defect you find at the end
GG25 has low tensile strength, so when the tool exits the part the unsupported material in front of it simply breaks away. It happens leaving a milled face, drilling through a hole and turning out to the end of a diameter. The fixes are cheap: reduce the feed on the last stretch, put a chamfer on the exit face, and orient the milling so teeth exit into material rather than into air. If the part is machined from both sides, plan the order so no critical edge is ever where the tool leaves.
Quick shop tips
First pass over casting skin: take 30% off the speed and get under the sand and oxide layer.
Mill dry; intermittent coolant cracks the insert in a comb pattern from thermal shock.
Protect ways and wipers: cast iron dust is abrasive and gets absolutely everywhere.
Halve the feed for the last millimetre of a through hole so the exit edge does not break out.
No form taps: cast iron does not flow and the thread comes out cracked.
On long continuous runs, look at ceramic or silicon nitride; they multiply the speed, but they demand absolutely dry cutting.
Frequently Asked Questions (FAQ)
Is grey cast iron machined with or without coolant?
Normally dry. Dust mixed with emulsion fouls the whole machine and, in milling, intermittent flood causes thermal cracking on the edge. Use extraction or air for the dust and save coolant for deep drilling or very tight tolerances.
Why do my edges chip out when milling GG25?
Because grey iron is weak in tension and unsupported material breaks away when the tooth exits the part. Reduce the feed at the exit, pre-chamfer the edge, and orient the toolpath so teeth exit into material wherever you can.
What Vc do I use on GG25 with an HSS drill?
Between 35 and 60 m/min with HSS, against 105-188 m/min for carbide. Cast iron drills well with HSS, but the abrasive dust wears the corners and the margin, so check hole diameters regularly.
Why does the first pass destroy my insert?
The casting skin: moulding sand, oxide and chilled areas full of very hard carbides. Enter at reduced speed, deep enough to get under that layer, and with an edge reinforced by a land.
Can I use GG25 parameters on ductile iron GGG50?
Not directly. Ductile iron is tougher and more ductile, makes a longer chip and wants 130-220 m/min. GG25 is more brittle and abrasive; GGG50 wears tools more through heat and adhesion.
