Aluminum Endmill Throwdown!! Destiny vs. Niagara vs. Gorilla vs. 2nd Shift Grinding - Page 2 - Practical Machinist - Largest Manufacturing Technology Forum on the Web

Gumby · #21 (**permalink**) 04-15-2009, 04:09 AM

Quote:

Originally Posted by Perry Harrington

I'm trying this cutter out at the recommendation of my local grinder, he has a lot of experience and says this guy is very sharp and knows his geometry. Agreed the price isn't cheap, but experience says the cheap tool isn't always the cheapest. If I can increase my cut speed by 50%, it's the cheaper tool. I'll report back after trying it against the MT cutters I have.

I am not saying the tool isn't any good... but the 4 flute tool I found on their website is specifically designed for steel and will require more hp/induce greater cutting forces when compared to a tool like the Gorilla Mill Silverback in the OP. It will also not be able to handle near the CLPT of a 3 flute tool. This I am very much certain of. The tool the OP used in the test was polished and obviously required the least HP to push compared to the other tested tools.

Perry Harrington · #22 (**permalink**) 04-15-2009, 12:04 PM

I understand 2fl, 3fl, and 4fl well, and I understand the coating isn't proper. However, if the machine doesn't seem to like 3FL endmills.

This machine likes the 4fl, and it was loving every minute of it. Yes, 4fl endmills are weaker than 3fl, and they have less area for chips. However, I tried a 3fl endmill exactly like the one above and it just plain sucked. The excessive pitch spacing between the variable flutes (1 big gullet and increasingly smaller) was causing the machine to vibrate badly and it ate up way more HP than a standard 2FL Al grind.

The fact is, this is a Haas VF-0 and it is what it is. I'm just trying to make the best of what I can with this machine. I'm not disappointed per say, but I'm just not used to how it works. I've been using a box/dovetail machine for the last 5 years and it's a different beast altogether. It "only" has 4HP, but it will push harder on tools bigger than 1/2 than the Haas will, and won't complain.

I couldn't run a 1/2 endmill at any rate in the older machine because a of a lack of SFM, so I used 3/4 tooling to get the SFM up. The newer machine can do the same work faster because I can get more SFM and need to remove less material to get at the part. I understand you want me to try a proper 3FL against the 4FL, and I am open to that, after I get a handle on what the 4FL will do.

Perry Harrington · #23 (**permalink**) 04-15-2009, 04:26 PM

I received the 1/2 endmill from MNI this morning. I took some pics with my cellphone. The land width is huge on these. There is no primary relief on the land, just one big land. This will definitely support the cutting edge better. The geometry is vaguely similar to a core drill. The offset of the flutes isn't to create a larger flute area, the roughing land is wider than the finishing land. The core is also very large, probably 5/16 on a 1/2 drill. For aluminum I suspect there will be less room for chips, but that may be mitigated by the chipbreaker. I may also order a 3fl just to try out, maybe a comparo between Gumby's gorilla mill and MNI's terminator.

PaulT · #24 (**permalink**) 04-15-2009, 04:46 PM

Perry, please keep posting your results. I'm also trying optimize the 6061 removal rate on an underpowered and not very rigid machine so I'm real interested in your comparisons.

When I get a chance I'm going to do a comparison like StreetSpeed did (adjust ipm until at 100% load) on the fanciest endmill I currently have, a Lakeshore carbide vari-flute against the Maritool 3 fluters I have been using.

I realized also we're both "subjects of the Terminator", my shop's in Brisbane, just south of San Francisco.

Paul T.

Gumby · #25 (**permalink**) 04-15-2009, 05:10 PM

Quote:

Originally Posted by PaulT

Perry, please keep posting your results. I'm also trying optimize the 6061 removal rate on an underpowered and not very rigid machine so I'm real interested in your comparisons.

When I get a chance I'm going to do a comparison like StreetSpeed did (adjust ipm until at 100% load) on the fanciest endmill I currently have, a Lakeshore carbide vari-flute against the Maritool 3 fluters I have been using.

I realized also we're both "subjects of the Terminator", my shop's in Brisbane, just south of San Francisco.

Paul T.

Paul shoot me a PM with your information and I will drop a tool in the mail for you to test.

Perry Harrington, check this out: It is the Gorilla Mills Sasquatch tool.

I wouldn't really worry about edge strength in aluminum. We've pushed the Silverback tools to the point where they stop cutting and start extruding metal and it didn't damage the cutting edge (sounds real bad though...)

Bruce Griffing · #26 (**permalink**) 04-15-2009, 05:50 PM

Is there really no rpm limit on some of these tools when cutting aluminum? I am going to put a 24k spindle on one of my machines - but it is only 4hp. It will of course develop the most hp at top speed. Could you really use a 1/2" end mill in Al at those speeds?

Gumby · #27 (**permalink**) 04-15-2009, 06:05 PM

Quote:

Originally Posted by Bruce Griffing

Is there really no rpm limit on some of these tools when cutting aluminum? I am going to put a 24k spindle on one of my machines - but it is only 4hp. It will of course develop the most hp at top speed. Could you really use a 1/2" end mill in Al at those speeds?

Yes you can run a 1/2" tool at those speeds and faster. Someone here on these boards was running a 5/8" tool at 16krpm and aiming to hit 18krpm. Boeing runs tools at significantly higher speeds but usually with a DLC... However if you are only developing 4hp at 24krpm you are probably going to need to run a smaller tool.

StreetSpeed · #28 (**permalink**) 04-15-2009, 06:28 PM

I had a video of a Mazak running a 5/8" at 40,000 RPM and 1800 ipm. Aluminum is awesome.

FYI, LakeShore is sending me their newest tool to run through the gamut. I shall amend the results on the first page as soon as its tested.

ARB · #29 (**permalink**) 04-15-2009, 06:34 PM

I think you are going to like the tool from LSC.

Bruce Griffing · #30 (**permalink**) 04-15-2009, 06:35 PM

If I get 5 cipm/hp, then a 1/2" end mill cutting 1/2" deep should work out to 80ipm at 4hp. That would be at the limit of the spindle - but is that possible/in the ball park?

Gumby · #31 (**permalink**) 04-15-2009, 07:01 PM

Quote:

Originally Posted by StreetSpeed

I had a video of a Mazak running a 5/8" at 40,000 RPM and 1800 ipm. Aluminum is awesome.

FYI, LakeShore is sending me their newest tool to run through the gamut. I shall amend the results on the first page as soon as its tested.

lol scraping the paint off with chips I am sure!

Quote:

Originally Posted by Bruce Griffing

If I get 5 cipm/hp, then a 1/2" end mill cutting 1/2" deep should work out to 80ipm at 4hp. That would be at the limit of the spindle - but is that possible/in the ball park?

That seems like a 5.5hp cut. If you reduce your stepover to .375" I think would put you much closer to a 4hp cut.

StreetSpeed · #32 (**permalink**) 04-15-2009, 07:17 PM

Here's the video. One of my favs:

http://www.youtube.com/watch?v=YG_A6gvOS24

Gumby · #33 (**permalink**) 04-15-2009, 07:28 PM

Quote:

Originally Posted by StreetSpeed

Here's the video. One of my favs:

http://www.youtube.com/watch?v=YG_A6gvOS24

I've seen that one before. That is some serious metal removal!

Mickey_D · #34 (**permalink**) 04-15-2009, 08:20 PM

Bruce - I think you are going to let the magic smoke out of the new spindle if you try to run like that. You might want to step down to a 3/8th or even 1/4" (which is what I have done to get rapid cuts on stuff that I don't totally trust the fixturing on) because I bet that spindle will only develop full power near full speed. A smaller tool will let you use more of the flute and give you longer life on cheaper tools.

Bruce Griffing · #35 (**permalink**) 04-15-2009, 08:43 PM

Micky_D
I would certainly not start out with that type of cut. I simply took 5 cuipm/hp and calculated it out at 4hp and 24k rpm. I don't know if the 5 cuipm/hp number applies at this rpm - that was really the source of my question. My reason for thinking about 1/2" is this - I am not yet sure what xy speeds I am going to get with low following error. It may turn out that 80ipm will be more attractive than a higher xy speed from that perspective. So it is really a question of how to best take advantage of the machine after the conversion is complete.

CarbideBob · #36 (**permalink**) 04-15-2009, 09:37 PM

Oh Street , look what you've started.

So far ZrN runs the best on Aluminum, Gee imagine that...... No TiB2 yet???

Gumby, don't know how to break this to ya but you could do better in AL if you'd learn how to use micron graded wheels for finishing your flutes.
Bob

Gumby · #37 (**permalink**) 04-15-2009, 10:21 PM

Quote:

Originally Posted by CarbideBob

Oh Street , look what you've started.

So far ZrN runs the best on Aluminum, Gee imagine that...... No TiB2 yet???

Gumby, don't know how to break this to ya but you could do better in AL if you'd learn how to use micron graded wheels for finishing your flutes.
Bob

lol I don't actually make them. I do know that the tool I took a picture of was finished with a 600grit wheel. The tool tested by Mark was polished.

doug6949 · #38 (**permalink**) 04-15-2009, 10:25 PM

I noticed nobody mentioned Minicut endmills. We've had good luck with them on our VF5.

Don't have the numbers with me, but I think we are slotting 0.6 deep in 6061 at 60-70 ipm with a 5/8 endmill.

wrustle · #39 (**permalink**) 04-15-2009, 10:50 PM

Quote:

Originally Posted by Perry Harrington

I had the opportunity to try 3 different mills in my 5HP Haas VF-0. I tried the MariTool 1/2 3FL TiCN coated mill, 1/2 4FL variable flute TiAlN coated mill, and a 3/4 3FL variable flute ZrN coated endmill from exkenna (made by some outfit in NY I think).

The starting parameters were 5500rpm, 60ipm, full width slotting, .240doc in 6061.

The 3FL 1/2 would run 5500rpm at 60ipm, but it sounded like a buzzsaw, a lot of vibration. The main problem with this was the helix angle didn't pull the chips out of the slot and I had chips packing behind and chip recutting on subsequent passes. Not great, but not bad.

The 3FL 3/4 would plain not run fer crap. I had to back the motor down to 5250rpm to gain some torque, and it would only run 45ipm without making the spindle rpm bounce. It sounded like a jackhammer cutting the material, and the finish was nothing to write home about. My Shizuoka seems to like this endmill though, plows through quietly, throwing chips like mad.

The 4FL 1/2 mill was beautiful, it ran pretty smooth, the machine was just happy as a clam at 5500rpm, 60ipm. I got the feeling that I could run it at 75 to 90ipm. It gave a nice and smooth finish on my .005 finish pass. This still has a "normal" helix, but more flutes and a better geometry to evacuate chips.

I'm expecting a new contender tomorrow. It's from a guy in SoCal that my local tool grinder recommended. He makes a 3fl and 4fl, I opted for the 4fl because of the previous tests. My machine doesn't like 3fl mills. The 4fl has 2 flutes with chipbreakers and 2 flutes with finish grinds. The flute geometry is offset, the flutes are like 70/120 degrees apart, so it is going to be interesting. They aren't cheap, a 1/2" 4FL 1-1/4 LOC coated with flat is $68, but if it performs well and holds an edge for a long time, I'll be sold. The company is MNI Tool, www.mnitool.com

Hi Perry,

I have a 1992 VF-0 and have no problem running Lakeshore Carbide End Mills in my machine. A while back I had some slides I was making and took some video. Below is the link for the video. You can see the chips pouring out the back of the slot like water out of a hose. Near mirror finishes on the side walls as well.

1992 Haas VF-0

5,500 RPM 67 IPM .500 WOC .250 DOC

Lakeshore Carbide .500" Dia. Variable Flute ZrN Coating 3 Flute 1.25" Flute Length

http://www.lakeshorecarbide.com/12va...uminumzrn.aspx

Milling Video

http://www.youtube.com/watch?v=wgLs_8KhrX8

Picture of finished part.

Best Regards,
Russ

Slater · #40 (**permalink**) 04-15-2009, 11:26 PM

Why dont you guys include Robb Jack end mills in your test? We have had great luck with their A1 series cutters on aluminum. Price is about the same and they are great quality.