Roughing small gear teeth in mill turn

[DanWillows]

Hey guys I'm looking for some advice on a job I'm running at the moment, it's a toothed pulley similar to the htd or supercharger belt profile and the root of the tooth is almost a 2.5mm rad. I've only got 1 form cutter to cut the teeth so I'm roughing out the teeth with a 5mm ball to try to extend the form cutters life. The issue is the pulleys are fairly long (80mm) and have 50 teeth so roughing out the teeth is fairly slow. I'm running the cutter at 1200mm/min and ramping down in 6 passes but it still takes at least 40min per part. I've got a fair few to do and I'd rather not have the machine tied up for weeks on this job, anyone got any ideas to make it faster? Ideally I'd use a 5mm CRB drill and drill 50 holes in the face of the bar then turn the od to final diameter, but the stock I've got is only 1mm bigger than the diameter of the finished part so that's not an option this time. I've got some 4 flute ball nose coming that the tooling rep claims handle slotting fairly well but I'm doubtful it'll last as long as the 2 flute I'm currently using. I've wondered about tilting the endmill at 30-45° around the lathe y axis (mill-turn machine with a rotating milling head - mazak integrex i400) and dragging the cutter away from the chuck at full depth, in my mind it should help with chip clearance and reduce the amount of work the centre of the tool has to do. Anyone tried this? Can anyone point to any reading I can do on the topic, a quick Google search doesn't turn anything up.

 

[guythatbrews]

Titling at 45 will be a huge gain. Then the 4 flute can make a difference. Plowing with the dead center of the ball mill is killing you.

Better yet use a convex radius cutter. More expensive but more, stronger teeth.

 

[DanWillows]

Titling at 45 will be a huge gain. Then the 4 flute can make a difference. Plowing with the dead center of the ball mill is killing you.

Better yet use a convex radius cutter. More expensive but more, stronger teeth.

Yeah I've also got a iscar multimeter t-slot cutter on the way, on paper it'll be slower than the ball nose but I'm doubtful the ball nose will be capable of the speeds the rep says it is, at least not for very long.
Am I right in thinking that the more I can tilt the cutter the better it'll work? I've got 7mm of flute length and I'm only going 2.4mm deep so I'm theory I can tilt it at 70° but I'd need to cut more clearance behind the gear to make that happen

 

[ViktorS]

The more you tilt the longer tool stickout to avoid tool holder hitting workpiece.
Also, more tilt means longer tool engagement, might eventually start to chatter.

But a 40-50 degree tilt is really helping a lot for ball mill life and preformance, I regularly do this with our integrex.
Calculate surface speed at smallest engaging diameter of the tool to get correct feed and chipload, then let her rip!

 

[guythatbrews]

Yeah I've also got a iscar multimeter t-slot cutter on the way, on paper it'll be slower than the ball nose but I'm doubtful the ball nose will be capable of the speeds the rep says it is, at least not for very long.
Am I right in thinking that the more I can tilt the cutter the better it'll work? I've got 7mm of flute length and I'm only going 2.4mm deep so I'm theory I can tilt it at 70° but I'd need to cut more clearance behind the gear to make that happen

Yeah I'd stick with 45*. The more tilt the more overhang along with longer engagement. Tilting will really improve the performance.

Is the Iscar cutter stagger tooth indexable?

I used to cut 1" serrated splines with the corner of an endmill. Don't remember how many teerh but a lot. It always seemed like it shoulda been quicker.

 

[Brian285]

Have you looked at Vardex’s website? They indexable gear cutters, and they (and others) have indexable threadmills, perhaps a thread form will fit in your gear tooth well enough to rough it, or perhaps clear it out enough to run another tool after it?