[Robot Dude]

Ok I tried to find the information on feeds and speeds on google, but everyone wants to talk about chip load, or they start at 1/8" tool size, or the rpm too slow, or they want to sell you a program... lol I am stuck. I found this chart on the Kyocera website. I am not sure what to do with the numbers or which ones to use. Nothing is labeled chip load.

I want to route out some parts from 0.050" thick 7075 aluminum. I'm using a Kyocera 1620-0625.094, stub length, 30° Helix Angle, 2 flute, un-coated carbide end mill. My machine can do in excess of 120ipm and my spindle will do 24krpm. I can do 2 or 3 passes, no hurry. I have air to the cutter tip. I know the sweet spot is narrow and I just need a good starting point. thanks

Attachment 313626

Attachment 313628

Attachment 313630

[Robot Dude]

I found this calculator. I will try 8.2ipm yee effin ha...

Attachment 313746

[rbest42]

Can pretty much max it out in rpm. Start with .0004 per tooth


Sent from my iPhone using Tapatalk

[louieatienza]

I'd do it in 2 passes at about 12krpm and about 18ipm. Also you have a spoilboard - do all the through holes first, then you can screw the plate down (use nylon washers if surface is a concern) then cut the perimeter and you won't have to do tabs. Finally, you have some oval holes. Sometimes the slug will fly out, sometimes they'll twist in the hole and jam the bit, which will snap it like a dry twig. I'd pocket all those larger holes with at least a 1/8"-3/16" endmill, and you can do that in one pass.

[Robot Dude]

Thanks Louie, I ended up doing a conservative 3 passes at 12krpm and 12ipm and it turned out well. I did that before I read your reply. I also think I can do it in 2 passes. I will try 12krpm and 18ipm next time.

Attachment 315280

Attachment 315282

[victorofga]

you could take loui advice about holding down...
fileing off those tabs , never be like a milled surface..

watching you video theres some resonance occur..
surface also shows that resonance.. mightbe a little kerosene, or wd40 could help.. mightbe shallowing passes.. not 3 but 4-5 ...

when I cut aluminum, I use pvc sheet under.. so particle board wont swelling up by coolant..

[Robot Dude]

Hi Victor, As I said I did my cuts before reading Louies post. I have some changes I want to make to the feed. I want to do two passes and speed it up a little. I do not want to do this is 5 passes... I also see no reason to use liquid coolant when the air is working so well. The tabs are not a problem for this application. Thanks for your comments.

[victorofga]

well

im glad youre satisfied with your result..

with hss tool you can achieve 350 sfm, with carbide tool almost 3000... ... that's why I tried to suggest higher federate and shallower passes..

instead trying to explain, I show you videos.. to see what is the difference between a mill and router..

heres two video, first is a similar built router like yours..... you can observe, he cuts shallow and way higher federate you did..
he also using coolant because coolant not only makes better surface, also reducing load on the machine..

in your video the sound and the picture you posted shows ""rigidity issue"" when I say lacking rigidity it means for wood pretty rigid, for aluminum is not..

another video a G0407 grizzly mill..
it also could be interesting for you, this mill you can get about $3000 and it cuts really metal
this mill has plenty rigidity compared with a router..

possible your spindle itself cost more than the whole grizzly mill with control...

it can take an inch deep pass..without resonance.. (vibration)

https://www.youtube.com/watch?v=fbWzqALUFjg


https://www.youtube.com/watch?v=aIygRynDR38

[deadlykitten]

Can pretty much max it out in rpm. Start with .0004 per tooth

Sent from my iPhone using Tapatalk

0.0004 "/z = ~0.01mm/z ? wtf ? this is not cutting, is dust sweeping ...

0.01mm/z will generate a cutting speed for grinding, not for cutting, and that speed is not measured in mm/z, but in M/min or M/s when rpm is really high ...

i really admire anyone who targets high_max_rpm and low_min_feeds ...


i am glad you have an iPhone

[rbest42]

0.0004 "/z = ~0.01mm/z ? wtf ? this is not cutting, is dust sweeping ...

0.01mm/z will generate a cutting speed for grinding, not for cutting, and that speed is not measured in mm/z, but in M/min or M/s when rpm is really high ...

i really admire anyone who targets high_max_rpm and low_min_feeds ...


i am glad you have an iPhone

I'm glad you have nothing better to do then troll in forums .

[deadlykitten]

Thanks Louie, I ended up doing a conservative 3 passes at 12krpm and 12ipm and it turned out well. I did that before I read your reply. I also think I can do it in 2 passes. I will try 12krpm and 18ipm next time.

depending on quantity you need to machine, you can also think process stability, so don't try only to obtain your parts, but know-how

more parts, more trial runs, and get your conclusions

now, your part :

0.05" = 1.27 mm ... hmm, looking at your spindle, at your machine, at broach size ... that collet size is a bit to close to your broach size, so you can go :
.... 2-3 passes with new tool, for a few times - this procees targets unique/small series
.... 3-4 passes with weared tools, for more times - this proceess targets more parts

[12...18ipm]/12krpm=[304.8 .. 457.2mm]/12krpm=0.025 .. 0.038 mm/rot=0.025 .. 0.040mm/rot

12krpm x [ 0.025 .. 0.040mm/rot ] = 300 .. 460 mm/min

your tool is Kyocera 1620-0625.094, so 1/16"=1.6mm
20 .. 30% of 1.6 is 0.32 .. 0.48mm, and this means 1.27/0.32 ... 1.27/0.48 = 3.96 .. 2.64 = ~ 4 .. 2.5 passes

you can go [2 rough][ (1.27-0.2)/2=0.535mm ] + 1 finish [ 0.2mm ], so to bump a little your machine
you can go [3 rough][ (1.27-0.2)/3=0.35mm ] + 1 finish [ 0.2mm ], so to bump a little less your machine
you can go [4 rough][ (1.27-0.2)/4=0.26mm ] + 1 finish [ 0.2mm ], so to protect tool and spindle

also, you may consider 300mm/min rough, and 400mm/min as finish ...

your machine specs : 24krpm, and 120ipm=3000mm, so go 16krpm, considering 65% of your max rpm

kindly !

one more thing :
....if you go [ 16k (o/min) ] x [ 0.025 (mm/o) ] = 400 mm /min
....if you go [ 16k x 0.8 (o/min) ] x [ 0.025 x (1/0.8) (mm/o) ] = 400 mm /min, so to target same time, wear will be different
....a weared tool can continue for a while with reduced rpm, and with feed±20% .... just listen to it

don't go 24krpm x 0.01mm/o ... target at least 0.020 .. 0.025

[victorofga]

deadly kitten

""just listen to it""

that was how we worked..
also we take to the grinder and sparks said what material is it...

im not so scientific.. I have thumb rule between 1-2 percent of dia per tooth.. ... I mean for finish and certain way the depth also shouldn't excedd 30 percent of tool dia...
for roughing can be more the depth..

im not sure if it were taught this way, but years will teach it you...

I agree very much about worn tool... partically what I saw in the worn state a tool still work very long time..

like your calculation..

===========================================
many folks still confused with differences between router and mill... that's why posted both example...