What's new
What's new

DOC Recommendation for .150 slot with .125 endmill?

gmoushon

Cast Iron
Joined
May 18, 2006
Location
Illinois
What would be an optimal DOC setting to cut a 0.150 wide slot that is 0.321 deep in 6061? Slot is open on one end.

Currently I'm taking a 0.040 DOC at 30ipm with good flood coolant. I have 130 of these to do and am wondering if I couldn't speed up the process quite a bit.

I'm using a 1/8 MariTool 3-flute ZrN endmill and max spindle on this VF2 is 7500rpm.

Any suggestions would be greatly appreciated.

gm.
 
Did you bother looking at their chart?

Thanks for the reply and, yes, I did bother to look. I was just a little confused about this line from the chart: "slotting depth of 1.0 x Cutting Diameter, for deeper slotting reduce feed and speed" Does this mean that the full depth of 0.321 can be taken by simply reducing the feed and speed? That just seemed a little too aggressive for an 1/8 cutter.

I was trying to avoid tool breakage approach as this is what I've done in the past.

Thanks again for taking the time to reply.
gm
 
Thanks for the reply and, yes, I did bother to look. I was just a little confused about this line from the chart: "slotting depth of 1.0 x Cutting Diameter, for deeper slotting reduce feed and speed" Does this mean that the full depth of 0.321 can be taken by simply reducing the feed and speed? That just seemed a little too aggressive for an 1/8 cutter.

I was trying to avoid tool breakage approach as this is what I've done in the past.

Thanks again for taking the time to reply.
gm

Well, according to their chart, you can go .125 deep at .0016" ipt. But since your max spindle speed is 7500, I'd probably back off a tad on the feed.
 
I am not sure how your machine reacts but you can use two feed rates, the first one would be for full engagement but the second feed I would double if not triple your feed out of the part.
 
I think the right answer is it depends on who is buying the tools. If it is your employer, go for it. If it is your machine and your tool cost .040" per pass is just fine.
 
I do a similar slot on my MM2. 6krpm, first slot .125" deep, 30ipm. Back off Doc to .0625 for subsequent cuts till hit finished depth.

I run lakeshore 3fl zrn alum finishers for this. I'd order another endmill or two and start upping Doc and feed.

Sent from my SM-G955U using Tapatalk
 
I think the right answer is it depends on who is buying the tools. If it is your employer, go for it. If it is your machine and your tool cost .040" per pass is just fine.

I'm gonna disagree with you there. If it's your tool and you're only using .04" of the flutes, the tool will be worn out 3x faster than if you'd gone deeper, because each corner will have plowed through 3x as much. The tips don't know if there's .03" above them cutting of .1" above them cutting, they just know they're taking nine passes where three would do.

There's a happy medium between stress at the root from deflection, which goes up with increased DOC, and wear at the tips which goes up with more passes. That's why speed and feed charts exist.

Of course, that's all assuming you can clear the chips. If you don't have good coolant flow, then that's its own whole topic.
 
We use Gwizard from cnccookbook.com to calculate speeds and feeds. In the 4 years or so that we've been using it we've never broken a single tool. I think it's around $250 for a lifetime subscription. It will pay for itself pretty quickly by not breaking tools.
 
I'm pretty conservative as we don't do much volume of anything.... I would connect the open end and do a ramp toolpath at about .02" 45ipm and about your max 7500 rpm. If you have the tool, use a 1/4" loc and get the ramp depth to .03-.04" at same rpm and 50-60ipm
 
I'm gonna disagree with you there. If it's your tool and you're only using .04" of the flutes, the tool will be worn out 3x faster than if you'd gone deeper, because each corner will have plowed through 3x as much. The tips don't know if there's .03" above them cutting of .1" above them cutting, they just know they're taking nine passes where three would do.

There's a happy medium between stress at the root from deflection, which goes up with increased DOC, and wear at the tips which goes up with more passes. That's why speed and feed charts exist.

Of course, that's all assuming you can clear the chips. If you don't have good coolant flow, then that's its own whole topic.

Umm.. it's aluminum, you aren't wearing the ends/tips off anytime soon

edit: we cut aluminum and brass every day and to *fine* detail, you aren't seeing any wear anytime soon...
 
Umm.. it's aluminum, you aren't wearing the ends/tips off anytime soon

edit: we cut aluminum and brass every day and to *fine* detail, you aren't seeing any wear anytime soon...

The only time I would see wear is if the tool is sticking out too far and there is vibration other than that it will take a long time to wear this tool out.
 
Did you bother reading his post? He says he is running 7500rpm. Probably a machine limitation. Maritool recommends 800spfm. That amounts to 24,446RPM. He will probably fail at recommended DOC since he can only cut at 245RPM. I would recommend 50% DOC.

Did you bother reading my post after that one?
 
All good points above. Other than the already mentioned stickout, my biggest concern when slotting close to a tools diameter is chip evacuation. Sometimes drilling or boring a hole at the closed end slightly undersized can help with chip flushing. Ramping into the slot can also be useful as well. But, as others have already said, you're running a pretty small slot depth in aluminum so you'll be fine with a wide swath of cutting parameters.

Go for as short a stickout as you can while still maintaining good flood coolant and you'll be golden.
 








 
Back
Top