What's new
What's new

Slotting advice on 9000 1/8 x 1.4 inch slots.

AlloyCraft

Plastic
Joined
Feb 26, 2020
HI guys the job I am working on requires alot of slotting in 6061, I need to make a total of 9000 1/8 inch wide X 1.4in long x.265 deep slots. Right now its looking to be around 12 minutes per part for just the slots using a ramping strategy with a 1/8 in endmill. I am looking for suggestions on how to speed things up with a bit. Right now I am doing .0009 per tooth @ 12k rpm and ramping at 3 degrees in .156 steps. I do have an 60,000 rpm NSK air spindle that I can use, but I dont know if it will be any faster due to low chip loads it can handle. I was thinking about using the Helical 84942 high feed endmill in the air spindle. Has anyone had luck with a high feed endmill in a air spindle?
 
Try a 3mm 3 flute Harvey Tools stub mill. Get a few to break finding out how hard you can push them. They are the toughest end mills for aluminum I know of. I bet you could do them in two steps at a 5 degree or more ramp. Tib2 coating is worth it but maybe not for the first 2 or 3 you break finding out how fast you can go. I found tthe coating was good for at least a 20% feed improvement slotting with a 3/16" end mill in productin. My nornal go to for this would be a corn cob mill but I don't know of any that small.
 
First I would say if you can access it use a key cutter, but
.125@ just over 2XD deep in 6061, I would just send it!

coolant/chip removal is key.

I have a bunch of production parts I run, 3/16" cutter .500+ DOC I run a 2 flute for clearance and chatter mitigation, max rpm is 10,000, sweet spot was 12IPM and that's in 7075.
 
1200 SFPM(could probably go faster) =36000RPM at .002 DOC ramping. I get 2 minutes 19 seconds per slot. Use your NSK, it should handle this very well. Plenty of coolant. Also, this is at .001 chip load with a 4 flute. 146IPM.
Edit: I forgot to mention, this time was for ramping in one direction. If you ramp in both directions the cycle time is 1 minute 13 seconds per slot.
 
Last edited:
Try a 3mm 3 flute Harvey Tools stub mill. Get a few to break finding out how hard you can push them. They are the toughest end mills for aluminum I know of. I bet you could do them in two steps at a 5 degree or more ramp. Tib2 coating is worth it but maybe not for the first 2 or 3 you break finding out how fast you can go. I found tthe coating was good for at least a 20% feed improvement slotting with a 3/16" end mill in productin. My nornal go to for this would be a corn cob mill but I don't know of any that small.
Thanks for the recommendation I will give them a try. Looking at this one particularly,

TOOL # 900457-C8​

 
What is the time per slot? Just for perspective on how far you can go.
I just received P.O. this morning so I haven't actually cut anything yet. But cam says 15 seconds per slot using the recipe in the first post. That would be a 1/8 3 flt endmill. With the air spindle and high feed endmill at 60k rpm .0035 ipt and 3 deg ramp and .0047 steps I get around 11 seconds per slot. However that puts the feed rate at 768 ipm! There are 46 slots per part.
 
Last edited:
Are they open ended slots, or closed.
ramping isn't a very good machining strategy, end mills don't like to cut on their ends, you can even listen to the difference.
if you can(open ended slots) and you need multiple depths, then drop in, straight through, then drop to the next level, ramping you will have a higher failure rate or chance.
 
HI guys the job I am working on requires alot of slotting in 6061, I need to make a total of 9000 1/8 inch wide X 1.4in long x.265 deep slots. Right now its looking to be around 12 minutes per part for just the slots using a ramping strategy with a 1/8 in endmill. I am looking for suggestions on how to speed things up with a bit. Right now I am doing .0009 per tooth @ 12k rpm and ramping at 3 degrees in .156 steps. I do have an 60,000 rpm NSK air spindle that I can use, but I dont know if it will be any faster due to low chip loads it can handle. I was thinking about using the Helical 84942 high feed endmill in the air spindle. Has anyone had luck with a high feed endmill in a air spindle?
Can a key cutter hit it? A shaft, or within reach of an edge?
Got a right angle head? Can you use a wheel?
I have done my share of these in 6061 with .0005 chip load at 8k RPM, and I don't remember my DOC.
A horizontal milling wheel blade or a keo cutter will kick ass on an end mill, if you can fit them.
 
Are they open ended slots, or closed.
ramping isn't a very good machining strategy, end mills don't like to cut on their ends, you can even listen to the difference.
if you can(open ended slots) and you need multiple depths, then drop in, straight through, then drop to the next level, ramping you will have a higher failure rate or chance.
Drill either end of the slot. Yeah, I tried ramping too, I was dying of old age.
 
I just received P.O. this morning so I haven't actually cut anything yet. But cam says 15 seconds per slot using the recipe in the first post. That would be a 1/8 3 flt endmill. With the air spindle and high feed endmill at 60k rpm .0035 ipt and 3 deg ramp and .0047 steps I get around 11 seconds per slot. However that puts the feed rate at 768 ipm! There are 46 slots per part.
The saw would smoke that all to hell.
How about .8 seconds, would that work?
Or, do you have a problem with making money?
 
Last edited:
Are they open ended slots, or closed.
ramping isn't a very good machining strategy, end mills don't like to cut on their ends, you can even listen to the difference.
if you can(open ended slots) and you need multiple depths, then drop in, straight through, then drop to the next level, ramping you will have a higher failure rate or chance.
Actually ramping works pretty well for me. It is center cutting end mills hate.


Don't know what machine, but if you have have a small drill being used, or can spare the tool change drill a clearance it will run faster if your toolchanger is faster
193 inches [3 passes 1.4 inches 46 slots] seems it ought to go faster even at 12k
 
The saw would smoke that all to hell.
How about .8 seconds, would that work?
Or, do you have a problem with making money?
Not seeing how a saw (key cutter, horizontal, etc) would make a finished slot. I think of slot being two half circles joined by two lines.
They can make a rectangle with beveled ends?
Drill mill.
 
Actually ramping works pretty well for me. It is center cutting end mills hate.

Don't know what machine, but if you have have a small drill being used, or can spare the tool change drill a clearance it will run faster if your toolchanger is faster
193 inches [3 passes 1.4 inches 46 slots] seems it ought to go faster even at 12k
ramping is OK, sometimes unavoidable, usually just lazy programming, but drilling a clearance hole as you mention, dropping to depth I find faster and more reliable, what I would consider better machining practice.

for new guys as a reference, noticing on a HSM tool path that the ramping is always slower than the to depth feed rate, shows that ramping is a slower MRR.

Not seeing how a saw (key cutter, horizontal, etc) would make a finished slot. I think of slot being two half circles joined by two lines.
They can make a rectangle with beveled ends?
Drill mill.
'slotting' is a milling strategy, not all 'slots' have closed ends. open ended slots will always be better/faster machined with key cutters.
unfortunately we almost never get a scenario where we can utilize it.
 
Are they open ended slots, or closed.
ramping isn't a very good machining strategy, end mills don't like to cut on their ends, you can even listen to the difference.
if you can(open ended slots) and you need multiple depths, then drop in, straight through, then drop to the next level, ramping you will have a higher failure rate or chance.
These are closed end obrounds slots so, its either drill a start hole or ramp in. I will try a drill hole strategy as well to see if it can improve cycle time.
 
Last edited:
These are closed end obrounds slots so, its either drill a start hole or ramp in. I will try a drill hole strategy as well to see if it can improve cycle time.
OK, I personally if your machine is fairly fast at tool change and not a dinosaur,
would drill one end under .125" , use 3mm EM drop in half depth, one pass, drop full final rough, if you can a single rough pass,
then finish around once for clean up.
 
OK, I personally if your machine is fairly fast at tool change and not a dinosaur,
would drill one end under .125" , use 3mm EM drop in half depth, one pass, drop full final rough, if you can a single rough pass,
then finish around once for clean up.
These are run on a 5 axis because the slots are on 4 sides and I have to touch all 5 sides. So it means only one part per cycle, but I think punching an 1/8 inch hole and then milling the slot in 2 depths will cut the slot time down to around 5-6 seconds each, well if everything works according the the tool manufacturer speeds and feeds. I found a cob style mill in 1/8 inch, Helical tool 87770. Supposed to be able to do .0007 ipt @ 75%-125% of dia depth full slotting, and I think it should handle .0009 ipt with a short stick out and a .135 ADC. Hole wall finish is not critical as these are just air holes so hopefully the cob mill will leave a decent enough finish. Thanks for the suggestions, I will update when I run the parts.
 
These are run on a 5 axis because the slots are on 4 sides and I have to touch all 5 sides. So it means only one part per cycle, but I think punching an 1/8 inch hole and then milling the slot in 2 depths will cut the slot time down to around 5-6 seconds each, well if everything works according the the tool manufacturer speeds and feeds. I found a cob style mill in 1/8 inch, Helical tool 87770. Supposed to be able to do .0007 ipt @ 75%-125% of dia depth full slotting, and I think it should handle .0009 ipt with a short stick out and a .135 ADC. Hole wall finish is not critical as these are just air holes so hopefully the cob mill will leave a decent enough finish. Thanks for the suggestions, I will update when I run the parts.
That isn't a corn cobb, that is a semi-finisher or chip breaker, similar,
these actually do leave a useable finish if not critical, unlike a corn cobb.

Also 2 flutes give more chip clearance, so if your breaking them try a 2 flute.
what is nice is if they have oversized shanks, then they break at the shank instead of in the collet.

shrink holders works well because you get good coolant access.

 
That isn't a corn cobb, that is a semi-finisher or chip breaker, similar,
these actually do leave a useable finish if not critical, unlike a corn cobb.

Also 2 flutes give more chip clearance, so if your breaking them try a 2 flute.
what is nice is if they have oversized shanks, then they break at the shank instead of in the collet.

shrink holders works well because you get good coolant access.

Love my shrink holders. Made a visible difference. I just use my turbo torch to change them. Just keep the heat fast, intense, and even.
Mine, spinning on a string...
 








 
Back
Top