Reducing cycle time when chamfering large parts

Captdave · Feb 26, 2017

Looking at reducing cycle time of chamfering, so looking at different tools to see if we couldn't make some improvements there. Currently were using a standard 4 flute 3/8" Mari chamfer tool just to cut a .025" chamfer to break an edge in 6061.

Currently running 12K 400IPM ~.009" FPT which gives an acceptable finish but running on a machine capable of feedrates up to 1500 IPM leaves a lot on the table when most parts have 20 to 30" linear inches of chamfer per side.

Most chamfer tools with more flutes like 8 or 10 are 1" or larger in HSS. So got to thinking about some of the 1/2" 8 flute EM from Mari and having maybe a .100" chamfer custom ground on the end and giving it a shot. I know there isn't much clearance between the flutes but I'm thinking for a .025" chamfer it shouldn't need much and kicking up the feed to maybe 800IPM or more.

What do you think?

.5 x 1.25 x 3. TiAlN Coated 8 Flute Finisher - Made in USA MariTool

implmex · Feb 26, 2017

Hi Captdave:
Since the limiting feedrate for a good finish will be governed by your flute count (and spindle speed), you're obviously right to look at flute count once you've maxed your spindle speed.
But the risk you increasingly run is that you pile chips up in a gullet and smear the crap out of your chamfer.
Have you looked to see if there are through tool coolant chamfer mills with high flute counts?
Would you consider having customs ground up for you from TTC endmills if there are not?

I'd still try to get the biggest tools that will fit your minimum part radius of course; just so you can get the biggest possible gullets even with lots of flutes.
Also if you really cannot get a suitable starting point from an existing endmill or can't buy an off the shelf TTC chamfer tool, would you consider having coolant channels hole popped into an endmill or a carbide blank.

I normally try to stay away from custom tooling especially elaborate custom tooling whenever possible, however I'm also willing to bet that many shops would be thrilled to be running their chamfers at 400 IPM and would scratch their heads and call you an idiot for wanting more, so I doubt you'll easily find an off the shelf solution.

A quick Google search found nothing suitable, but I may have overlooked something.
I'm sure AB Tools would happily grind you up something suitable from a Maritool cutter, a gazillion shops can holepop them for you and since you're cutting aluminum, you should get the tool life to justify the cost if you can really gain worthwhile amounts of time.
I don't think I'd be brave enough to try without high pressure TTC aimed right at the chamfer from inside the tool...I don't think you have the gullet space for it at 12K RPM with 8 flutes and only a 1/2" diameter cutter at 800 IPM, but obviously I'm guessing here because I've never tried it.

Cheers

Marcus
Implant Mechanix • Design & Innovation > HOME
www.vancouverwireedm.com

Winterfalke · Feb 26, 2017

My standard chamfer tool list was a 1/4" 4 flute with 45deg corners for small internal corners (we had them on hand for some other job), a Coromill EH 3/8 shank holder with a .675" 45 degree 6 flute keyslot type head for fast outside profiling, and a Coromill EH 1/2 shank with a 1/2 45deg 8 flute chamfer tool with the tip flatted for kind of universal deburring. I have used a carbide rotary burr with some success, I think it had like 28 flutes and worked reasonably well with a lower IPR, but I could feed faster. More flutes are better, I think the 8 flute EMs would work great with a 45deg corner added, my biggest problem is getting high flute count tooling with an aluminum appropriate grind.

SND · Feb 26, 2017

Could be worth a shot, surely one of the members here that do endmill regrinding could do that mod, or maybe Frank can just special order that for you since he already sells them in 4 flute chamfered.

There's a few factory options with 5 and 6 flute in the 3/8 and 1/2" size.

Captdave · Feb 26, 2017

implmex said:
Hi Captdave:
Since the limiting feedrate for a good finish will be governed by your flute count (and spindle speed), you're obviously right to look at flute count once you've maxed your spindle speed.
But the risk you increasingly run is that you pile chips up in a gullet and smear the crap out of your chamfer.
Have you looked to see if there are through tool coolant chamfer mills with high flute counts?
Would you consider having customs ground up for you from TTC endmills if there are not?

I'd still try to get the biggest tools that will fit your minimum part radius of course; just so you can get the biggest possible gullets even with lots of flutes.
Also if you really cannot get a suitable starting point from an existing endmill or can't buy an off the shelf TTC chamfer tool, would you consider having coolant channels hole popped into an endmill or a carbide blank.

I normally try to stay away from custom tooling especially elaborate custom tooling whenever possible, however I'm also willing to bet that many shops would be thrilled to be running their chamfers at 400 IPM and would scratch their heads and call you an idiot for wanting more, so I doubt you'll easily find an off the shelf solution.

A quick Google search found nothing suitable, but I may have overlooked something.
I'm sure AB Tools would happily grind you up something suitable from a Maritool cutter, a gazillion shops can holepop them for you and since you're cutting aluminum, you should get the tool life to justify the cost if you can really gain worthwhile amounts of time.
I don't think I'd be brave enough to try without high pressure TTC aimed right at the chamfer from inside the tool...I don't think you have the gullet space for it at 12K RPM with 8 flutes and only a 1/2" diameter cutter at 800 IPM, but obviously I'm guessing here because I've never tried it.

Cheers

Marcus
Implant Mechanix • Design & Innovation > HOME
www.vancouverwireedm.com

It just happens that I'm installing TSC on this machine this week, just pulled the power for it yesterday and the pump should be here later this week.
Mari has been pretty fair about doing some custom grinds for us in the past so I might give them a call and run it by them and see what they think, who knows they may have a better solution that we haven't thought about. Perhaps a 6 flute would be a better choice and I have no problem spending a couple hundred just to give it a shot, either it works or doesn't, either way I can cross it off the list and get it off my mind!

Shop Supply Guru · Feb 26, 2017

Helical has standard 5 flute with helical flutes.

Helical Solutions - Chamfer Mills - Helical Flute, 3 & 5 Flute - High Performance

guest · Feb 26, 2017

Captdave said:
...What do you think?

What will be the improvement in throughput by cutting 2 seconds off the tool?

SND · Feb 26, 2017

For 6 fluters and what "should be" decent coolant access/chip flush I'd likely look more into a double angle chamfer tool... like this sorta thing for image purpose.

Harvey Tool - Double Angle Shank Cutters In Stock with Same-Day Shipping

DavidScott · Feb 26, 2017

I would like to hear what you find out since I do a lot of chamfering on aluminum and plastic parts as well and can feed much faster than the tools allow. The Helical/Harvey tools are 3 flute under 3/8" diameter. It would be nice to see a tool just for this type of work. I have seen Harvey Tool ask if there are tools they should look into making, perhaps this would be a good one for them. MA Ford makes some 6 flute chamfer tools at least down to 3/16" but they are not very special and don't work well on aluminum.

dstryr · Feb 26, 2017

Destiny makes a really nice helical 3 flute chamfer mill for aluminum but I'm not chamferinng at 400 ipm either LOL

Seems kinda like a waste of energy to look into this when the total savings is going to be very small?

DavidScott · Feb 26, 2017

SND said:
For 6 fluters and what "should be" decent coolant access/chip flush I'd likely look more into a double angle chamfer tool... like this sorta thing for image purpose.

Harvey Tool - Double Angle Shank Cutters In Stock with Same-Day Shipping

They could do a hell of a lot better than that if they tried. I just got a 3/16" diameter 5 flute profile mill for aluminum from them and it is a work of art. Just grind this type of flute allowing up to a .035" or so chamfer and as many cutting edges as they can put on the tool.

Ox · Feb 26, 2017

guest said:
What will be the improvement in throughput by cutting 2 seconds off the tool?

Well, someone beat me to the math.
Did you happen to run the numbers yourself?

No way that you (I, anyway) want to deal with specials for both availability and cost porpoises, to save 2 seconds/side of your (my) part.

This is piss poor ROI.

-------------------------------

Think Snow Eh!
Ox

implmex · Feb 26, 2017

C'mon guys
At this point only Dave knows what his part geometry actually is; there could be a gazillion ribs to chamfer for all we know.
He thinks it's worthwhile to try to make gains here; why should we piss and moan about what a dumb idea it must be without even knowing what the part looks like.
The big question is still whether he can find a way to double his feedrate on these chamfers and still get a good part.
I can't see how it's our business to question that.

Cheers

Marcus
Implant Mechanix • Design & Innovation > HOME
www.vancouverwireedm.com

Tonytn36 · Feb 27, 2017

Ox said:
This is piss poor ROI.

Hrm... not really.....

That 2.25 sec is 37.5 minutes over 1000 parts which is $2,437.50 @ $65 shop rate. Not a bad return on a $200 EM. (ASSuMEing the EM lasts 1000 parts, which in 6061 is very likely, especially if he has the 45° ground wide long enough to double or triple use it by moving his depth when dull.)

NodecoMachine · Feb 27, 2017

These have 12 teeth... I personally haven't used them but Harvey knows there shit. Sounds like what you want. Maybe a larger dia. custom?

gustafson · Feb 27, 2017

Tonytn36 said:
Hrm... not really.....

That 2.25 sec is 37.5 minutes over 1000 parts which is $2,437.50 @ $65 shop rate. Not a bad return on a $200 EM. (ASSuMEing the EM lasts 1000 parts, which in 6061 is very likely, especially if he has the 45° ground wide long enough to double or triple use it by moving his depth when dull.)

umm umm umm

I see 40 bucks, as in 37.5 minutes is a fraction of a 65 dollar hour

so payoff is like 5000 parts to breakeven

Captdave · Feb 27, 2017

So I checked the CAD on the parts currently on the machine and the OP10 has 43 linear inches X 5 parts and OP20 has 36 linear inches x 5 parts for a total of 405" per cycle x ~330 parts per day = 13,365" of chamfer. I think this is a good average, some parts have more and some have less.

I'm not looking to drop minutes of each cycle, but given that every part we machine has to be chamfered I at least wanted to visit the subject and see if there was any better tooling options and if there was any room for improvement.

Scruffy887 · Feb 27, 2017

Next big question. You can program the feed much faster but will the machine actually feed that fast? Part complexity will play a big role here as accel and decel feeds in corners add up. For me to go forward I would time the present cycle, remove part and change feed, then cut some air with existing tool and time that cycle.

gustafson · Feb 27, 2017

That's definitely some time there

While I cannot help but think that there are other places that will save more time, have you considered a spindle speeder?

Basically you are out of spindle speed and since it is a non wear item[essentially] it would amortize over quite a few parts, especially if you had some other use for it[say drilling some small holes]

Captdave · Feb 27, 2017

The majority of our parts are round 4-6" OD 3" ID and some 1.25" counter bores. I'm not sure the machine could feed much faster in the counter bores with a larger tool but I'm pretty sure it will everywhere else.

Reducing cycle time when chamfering large parts

Titanium

Diamond

Stainless

Diamond

Titanium

Hot Rolled

guest

Guest

Diamond

Diamond

Diamond

Diamond

Diamond

Diamond

Diamond

Cast Iron

Diamond

Titanium

Titanium

Diamond

Titanium

Similar threads