[ryanschmidt224]

The title pretty much explains it but im having to slot a disc rotor made of 4130 and am cutting slots in it that are .07ish wide .25 deep and around 6inches of slotting per part... 60 parts.... an 1/16 e.m. is lasting around a whole 1 part. have tried several depths of cut and several fds/spd with several diff types of e.m's... any ideas?
Thanks
Ryan.

[HuFlungDung]

Predrill an entry point, so that you don't suffer endmill damage attempting to plunge into the cutting depth.

Rough with a stub length flute, coated carbide, 20000 rpm. I'd probably try to rough that out with sidewall 'draft', which would imply a slight angle inwards to create clearance for the rougher as it gets deeper into the work, so that the neck of the cutter does not rub. Set up your CAM so that each pass is about .001 narrower, at about .03" depth per pass.

Switch to a finishing tool and take two passes .125" deep to straighten up the wall. Keep in mind that the first .030" of the rougher gets dulled, so it won't do much of a job trying to finish at .125" deep, due to deflection of the dulled flutes.

If feasible, plan a rotation of the slightly worn finisher into the roughing routine, and then get a new finisher.

[ryanschmidt224]

there is a 2 inch pocket in the center so the predrill isnt a problem and i have just been grinding down endmills to releave the shank... i like your idea alot more with the .001 stepover. I am using a .03 depth currently but am running on a 7500 rpm machine. I was thinking about putting it on a 12000rpm instead but thats as high as we go. will i break down my tools fast if i ramp in on the slot? We have a big tolerance on the slot .030 so we are currently just running down than rapid up and back than doing it over, not feeding in, over, than out. Is there a certain type of e.m. you would reccomend?
Thanks,
Ryan

[HuFlungDung]

This kind of work is a good application for a spindle speeder: you can run high rpms without running the main spindle so desperately fast, whilst doing so little metal removal

It would also be essential to use an air blast, IMO, because its difficult to clear the flutes of those tiny endmills in full width cutting, so chip recutting can be a contributor to short tool life.

You could ramp in, although this might add significant length (and time) to the toolpath if you ramp in to a level, machine it level, then begin ramping again, while the tool is probably going to be running at a conservative feedrate no matter what. One trick I sometimes use with my cadcam is to use a boundary ramp entry the whole depth of the pocket, perhaps with an .047" or a 1.5mm endmill. I'll pick a ramp angle such that the descent rate is about .03 to .05 per orbit of the pocket (judged by how hard its working ).

I don't have a particular endmill preference. That is fairly routine material to cut, so I'd probably use a TIN or AlTIN coated from Harvey tool because I've got their catalogue , and its got a real nice selection of small tools so you can find just the optimum size and length to suit what you imagine for your best operational procedure.

[msomerville]

If you have .03 to work with I might think about stepping up to a 2mm e.m., but you should be able to do it with a 1/16 e.m.

[MarkieMark834]

make sure your endmill is built on a 1/4 or 3/16 shank. there are alot of applications where you need this style of geometry i will attach a picture so you can see. i have alot of customers who are doing what u are trying to do and this has been real succesful. If you are interested i can get you some more info.

[Mcgyver]

hehe, all you guys who threw away your horizontal mills - piece of cake in one pass. A tiny end mill can't compete - it just doesn't have the support...have you a horizontal?, maybe outsource to someone who does? A straight/slitting cutter in a stub arbor in a vertical might work if the disc dia isn;t so large that you can't reach all of it. if the slots aren't dead ended, ie they come out to each edge, here's a real time warp for ya - easy work for a shaper