Need tips using single flute router bits in 6061

Jrill · Sep 23, 2019

I bought a few different styles of single flute router bits from LMT Onsrud, ones specified as for aluminum, but they keep breaking. I've been using them at 4-8k rpm in VMCs, not in a real router spindle. I'm wondering how others use 1 or 2 flute router bits in aluminum, what works and what doesn't.

It seems like they're designed for high rpm, high doc, and really low chipload. Maybe they're designed to look cool and promptly break upon use? Seems like it sometimes.

Is cutting through 6061 0.125 extrusion with a 0.078-0.125 diameter single flute unrealistic?

D.D.Machine · Sep 23, 2019

look at YG-1 alu-power
There "WAY" cheaper than onsrud and do a great job in alum and plastic ,,, there is a lot of sellers on ebay that carry them.

for 1/8" extrusion i would go with a 1/4" dia and run max RPM ... just up your feed 5% at a time tell you snap a cutter then lower it by 20% and make parts,,, I get months and thousands of pounds of chips out of there 1/2" cutters and even get weeks out of the smaller cutters ...

guest · Sep 23, 2019

Jrill said:
...Is cutting through 6061 0.125 extrusion with a 0.078-0.125 diameter single flute unrealistic?

How fast are you feeding?

I don't use those single flute cutters, I use standard garden variety 2 fluters. I cut a shitload of extrusion. .120 wall 6005 (which cuts just like 6061). Job on the mill right now, I'm slotting with a 1/8" HSS cheap-as-dirt double-ender, loafing along at 6000 and 15 ipm.

That end mill has cut at least 800-1000 parts, still going strong...

garyhlucas · Sep 23, 2019

Can’t see a single flute that size being useful with only 8,000 rpm. 30,000 is closer to what you need.

Jrill · Sep 23, 2019

garyhlucas said:
Can’t see a single flute that size being useful with only 8,000 rpm. 30,000 is closer to what you need.

This makes a lot of sense. I figured that the extra flute clearance would be better somehow, but when you said that it suddenly occurred to me that yeah it would be great at 30k, but the cons outweigh the pros at lower rpms.

Jrill · Sep 23, 2019

guest said:
How fast are you feeding?

I don't use those single flute cutters, I use standard garden variety 2 fluters. I cut a shitload of extrusion. .120 wall 6005 (which cuts just like 6061). Job on the mill right now, I'm slotting with a 1/8" HSS cheap-as-dirt double-ender, loafing along at 6000 and 15 ipm.

That end mill has cut at least 800-1000 parts, still going strong...

So you're just using HSS at 6000 and it's working fine? How deep are you cutting, and do you have a hard time controlling deflection (1-2 finishing passes enough)? I've very rarely used hss 1/8 2fl end mills and I didn't realize they'd last so long.

guest · Sep 23, 2019

Jrill said:
So you're just using HSS at 6000 and it's working fine? How deep are you cutting, and do you have a hard time controlling deflection (1-2 finishing passes enough)? I've very rarely used hss 1/8 2fl end mills and I didn't realize they'd last so long.

Click on the pic I posted. That little notch in the end of the extrusion is the cut. It's 1-1/2" long and finishes .140" deep (wide?), measured from that end. So it's a full width slot with the 1/8" end mill, and a little slice, .015" thick falls off. The notch is relief for the plate that attaches to that end of the extrusion.

I take it in one pass, with a spring pass at 30ipm for good measure. Feed in, feed across, feed out. The extrusion is .120" thick, I program the Z depth at -.350". The flute length is 1/2", and Z0 is the top of the part. So there's only .030" of flute above the surface of the extrusion.

No deflection since it's a 3/8" shank cutter. If it starts pulling a burr, I can move it up to a fresh part of the flute. Do that once, use it up, and swap to the other end of the cutter and start over. Lasts forever.

I prefer HSS at the slow spindle speeds because it's more forgiving. I could run it faster, but have nothing to gain, since the machine is waiting on me anyway- short cycle part, 3 tools. While the machine is cutting, I'm setting the rivnuts and prepping the next part. In the time it takes me to do that, the part on the table is finished.

I use HSS exclusively on that extrusion. It lasts forever and it's cheap. If I was running long cycle times, I would use carbide and run a lot harder.

Wsurfer · Sep 24, 2019

Jrill said:
This makes a lot of sense. I figured that the extra flute clearance would be better somehow, but when you said that it suddenly occurred to me that yeah it would be great at 30k, but the cons outweigh the pros at lower rpms.

My understanding, since routers run such high spindle speed, they can't feed fast enough for a decent chip load, they would just rub and create more heat.
+1 on the yg-1. Crazy sharp

macgyver · Sep 24, 2019

I cut some 0.080 sheet on my cnc router, not sure the alloy but it was gummy to cut. I had trouble with it and the guys here said to get an onsrud cutter. I don't recall the part number, can find it if you need it when I get to the shop. Anyway, pulled up a test program but not 100% if I ended up here on the job but the test shows I started at 14,000 rpm and a feedrate of 25 ipm. The cutter was carbide single flute upshear. It worked really well on a full days worth of cutting and is still sharp and in very good shape. I did put a mister on it, but no flood coolant. Came off no burrs ready to go to finishing. All the other cutters I tried just gummed/welded up and made a mess.

Hope that helps some,
Jason

Jrill · Sep 24, 2019

D.D.Machine said:
look at YG-1 alu-power
There "WAY" cheaper than onsrud and do a great job in alum and plastic ,,, there is a lot of sellers on ebay that carry them.

Wsurfer said:
My understanding, since routers run such high spindle speed, they can't feed fast enough for a decent chip load, they would just rub and create more heat.
+1 on the yg-1. Crazy sharp

Which list of YG1 are you guys talking about? I'm using YG1 right now in the shop but I'm not all that familiar with all their styles

Jrill · Sep 24, 2019

macgyver said:
I cut some 0.080 sheet on my cnc router, not sure the alloy but it was gummy to cut. I had trouble with it and the guys here said to get an onsrud cutter. I don't recall the part number, can find it if you need it when I get to the shop. Anyway, pulled up a test program but not 100% if I ended up here on the job but the test shows I started at 14,000 rpm and a feedrate of 25 ipm. The cutter was carbide single flute upshear. It worked really well on a full days worth of cutting and is still sharp and in very good shape. I did put a mister on it, but no flood coolant. Came off no burrs ready to go to finishing. All the other cutters I tried just gummed/welded up and made a mess.

Hope that helps some,
Jason

What diameter were you using? Also do you have delamination problems with mist coolant? We run a lot of sheet that we tape down with double sided tape, but never tried to use mist on it. I did have a handful of good experiences with them but most of the time I was disappointed, glad to hear you had a good experience with them.

Jrill · Sep 24, 2019

guest said:
Click on the pic I posted. That little notch in the end of the extrusion is the cut. It's 1-1/2" long and finishes .140" deep (wide?), measured from that end. So it's a full width slot with the 1/8" end mill, and a little slice, .015" thick falls off. The notch is relief for the plate that attaches to that end of the extrusion.

I take it in one pass, with a spring pass at 30ipm for good measure. Feed in, feed across, feed out. The extrusion is .120" thick, I program the Z depth at -.350". The flute length is 1/2", and Z0 is the top of the part. So there's only .030" of flute above the surface of the extrusion.

No deflection since it's a 3/8" shank cutter. If it starts pulling a burr, I can move it up to a fresh part of the flute. Do that once, use it up, and swap to the other end of the cutter and start over. Lasts forever.

I prefer HSS at the slow spindle speeds because it's more forgiving. I could run it faster, but have nothing to gain, since the machine is waiting on me anyway- short cycle part, 3 tools. While the machine is cutting, I'm setting the rivnuts and prepping the next part. In the time it takes me to do that, the part on the table is finished.

I use HSS exclusively on that extrusion. It lasts forever and it's cheap. If I was running long cycle times, I would use carbide and run a lot harder.

Very good to know, thanks. We do a lot of 1/8" extrusion, small lot sizes but many different iterations, and I'm trying to find a good way to cut it all with a smaller tool instead of using a 1/4" and then cleaning up with an 1/8", or a 5/64", and etc.

guest · Sep 24, 2019

Jrill said:
...I'm trying to find a good way to cut it all with a smaller tool instead of using a 1/4" and then cleaning up with an 1/8", or a 5/64", and etc.

Going to 1/8" as a general purpose cutter isn't gonna be very good. The only time I use smaller than 1/4" is when the profile requires it. If there is any internal structure like ribs or webs, the 1/8" will snap like a twig. As long as there's nothing to run into on the underside, and you aren't using the bottom of the cutter, it's easy-peasy.

Obviously you have to hold the extrusion so it doesn't chatter- that's a big cutter killer, along with rubbing. You have to be cutting to keep your tool sharp.

1/4" or 3/8" are ideal for profiling cutouts. You will more than make up for the tool change with the higher chipload. And you don't need an entry hole, you can just plunge it through at 10ipm and go to town. I use YG's also.

Wsurfer · Sep 24, 2019

Jrill said:
Which list of YG1 are you guys talking about? I'm using YG1 right now in the shop but I'm not all that familiar with all their styles

Go to suncoast tool and select yg1 3 flute carbide, then alupower.then you can select diameter, length of cut etc.

guest · Sep 24, 2019

Jrill said:
Which list of YG1 are you guys talking about? I'm using YG1 right now in the shop but I'm not all that familiar with all their styles

1/8", I'm using YG1 EDP 11289. Think I paid about $12-$14 ea. from Western.

3/8" LOC, I mistakenly said 1/2" earlier...

macgyver · Sep 24, 2019

I remembered to look while at the shop. I used a 65-023 it is 1/4" dia. Looks like I dialed into 10,000 rpm at 30 ipm to run them out.

I assume you are asking about delamination of the mdf spoil board? If so, yes by the time the job was done the mdf was not in great shape. I was still able to use it for some other stuff, but I figured it in the job. I think the only reason I had to use the mister was the alloy, it was so gummy that without it I had lots of trouble. I would bet that a better alloy could run dry with that cutter. The customer supplied the material and he just bought the cheapest 4x10 sheet he could get and it cut like it.

Search

Largest Manufacturing Technology Community on the Web

Search

Need tips using single flute router bits in 6061

Jrill

Aluminum

D.D.Machine

Stainless

guest

Guest

garyhlucas

Stainless

Jrill

Aluminum

Jrill

Aluminum

guest

Guest

Wsurfer

Cast Iron

macgyver

Stainless

Attachments

Jrill

Aluminum

Jrill

Aluminum

Jrill

Aluminum

guest

Guest

Wsurfer

Cast Iron

guest

Guest

macgyver

Stainless

Similar threads