[tbev]

For an 1100, 5k MAX RPM. What's receive favorite cutter, fastest material removal. I'm looking specifically for interpolation. I'm currently hogging out parts at 5k RPM, 0.375doc, 0.075woc @100ipm. That's the most removal I have pushed it too so far, there's a bit of load but it's not bad and using adaptive tool paths it's running pretty nicely but I'm looking for more, maybe a corn cob rougher, currently using a 3fl, 45° helix CrN or TiCN,coated, (I think it's TiCN, it's capable of a little faster ipm than the CrN, which I didn't think would be the case)Tormach end mill. Thinking about a Keyocera insert cutter or some kind of corn cob, gotta stay@ .5 diameter or less, any recommendations are appreciate. . Happy New Year everyone!!

[wtopace]

For an 1100, 5k MAX RPM. What's receive favorite cutter, fastest material removal. I'm looking specifically for interpolation. I'm currently hogging out parts at 5k RPM, 0.375doc, 0.075woc @100ipm. That's the most removal I have pushed it too so far, there's a bit of load but it's not bad and using adaptive tool paths it's running pretty nicely but I'm looking for more, maybe a corn cob rougher, currently using a 3fl, 45° helix CrN or TiCN,coated, (I think it's TiCN, it's capable of a little faster ipm than the CrN, which I didn't think would be the case)Tormach end mill. Thinking about a Keyocera insert cutter or some kind of corn cob, gotta stay@ .5 diameter or less, any recommendations are appreciate. . Happy New Year everyone!!

What kind of material?

I would steer clear of the corn cob style on the 1100. I have one for aluminum and another TiAln for steel - both from Maritool. The aluminum one is usable, but very loud. The steel cutter is borderline unusable, my MRR goes way down (compared with a nice variable helix high performance endmill) and I have to tighten the power drawbar beyond what the bellville washers can do just to keep it from pulling out. If we had a more rigid machine, it might be a different story, but I can't get anywhere near my 1.5 HP with corn cob roughers.

Feel free to check out my short videos on instagram of me cutting 1018 steel at ~1.5 MRR with 3/8" variable helix endmills from onlinecarbide.com (no affiliation, just a happy customer). Personally, I don't feel like we have enough rigidity to rough with a 1/2" endmill effectively - I aim for 3/8" when trying to get rid of metal.

I feel like the modern geometry / HP endmills are so much better than the old style roughers that beat up the machine.

[CadRhino]

I have been using the Maritool 1/2" corn-cob rougher for aluminum on my 1100 the last three years and it is amazing. I first saw it used by John on NYC cnc videos.

What kind of material?

I would steer clear of the corn cob style on the 1100. I have one for aluminum and another TiAln for steel - both from Maritool. The aluminum one is usable, but very loud. The steel cutter is borderline unusable, my MRR goes way down (compared with a nice variable helix high performance endmill) and I have to tighten the power drawbar beyond what the bellville washers can do just to keep it from pulling out. If we had a more rigid machine, it might be a different story, but I can't get anywhere near my 1.5 HP with corn cob roughers.

Feel free to check out my short videos on instagram of me cutting 1018 steel at ~1.5 MRR with 3/8" variable helix endmills from onlinecarbide.com (no affiliation, just a happy customer). Personally, I don't feel like we have enough rigidity to rough with a 1/2" endmill effectively - I aim for 3/8" when trying to get rid of metal.

I feel like the modern geometry / HP endmills are so much better than the old style roughers that beat up the machine.

[tbev]

Aluminum, sorry I left that out.

Sent from my SM-G900V using Tapatalk

[tbev]

Do you guys know anymore details about the corn cobs your using, maybe we can figure out what works and what doesn't. I hear ya Wes, regarding the 3/8 vs 1/2 and the lack of power. If I could get a 3/8 Rougher to remove material a fast as the 1/2 I'm currently using I'd be stoaked!!

Sent from my SM-G900V using Tapatalk

[wtopace]

Do you guys know anymore details about the corn cobs your using, maybe we can figure out what works and what doesn't. I hear ya Wes, regarding the 3/8 vs 1/2 and the lack of power. If I could get a 3/8 Rougher to remove material a fast as the 1/2 I'm currently using I'd be stoaked!!

Sent from my SM-G900V using Tapatalk

If I did much aluminum there would be no competition - shear hog! Even nyccnc moved away from his corn cob for aluminum and went shear hog. Tormach sells one with the tts shank for a good price.

[tbev]

Agreed, I have a .75 shear hog, is bad ass. I've been comparing roughing with the shear hog vs. half in em but in this particular case I have to finish/rest machine with a 3/16in end mill, which is really the crocks of my problem with this particular part. Going from the shear hog leaves so much more material for the 3/16 bit to remove it takes a good amount more time to complete the past than the half inch em filter by the 3/16. I also threw a 1/4in bit in the middle (rough with shear hog, follow up with 1/4in em then finish with 3/16 em) but it's not really worth it with the additional tool change required, especially with my super cool lack of an ATC..

So I'm back to looking for a better half inch diameter cutter. . I'm also going to see what I can get my new 3/8in. 3fl, INCO Streaker to do. If I can get it to remove material as far or faster it will be awesome. You really prefer the 3/8 em to a 1/2 em on the 1100 huh? I hope it works for me too! John Grimsmo told me to get a Streaker, he really likes a 1/4in on his 1100 so I grabbed s coupe of those, in 3/8in tho bc that's what I needed at the time.

Does anyone use an insert cutter/ indexable in a half in, in aluminium? Again, I love the hog, but I'm not sure about a half inch version, I know AB doesn't make one but Keyocera does, I'm thinking about it.

BTW, I have a few chamfer bits I got from onlinecarbide.com that I really like, they were like $8/ea, they are great. I've also been using icarbide 's stuff, it's all fantastic too, 10pk of superfly inserts are like $30! [email protected] will take care of you for those if you tell him I sent ya. I met him at faves a couple years ago and he's real cool, good parts.

Sent from my SM-G900V using Tapatalk

[RussMachine]

I use 1/2" HSS Rougher Endmills in Aluminum on my 1 HP 770 all the time.
I run them at 5000 RPM, .687" depth of cut, with a .150 step-over.
Feedrate is a little slow at 18 IPM, but that's because of my Full-Depth cut. I don't like stalling the motor.
I also use flood coolant.
One endmill lasts me along time.

[cobrakai]

I have been using a Lakeshore 1/2" 3FL "finisher/rougher" with ZrN coating. I use it for roughing and finishing. It hums along very silently, shooting a steady stream of aluminum chips.

I was going to try a corncob cutter next, but these comments are kinda scary. I thought the serrated edge is supposed to increase MRR and reduce vibration/harmonics/noise?

[tbev]

I have been testing that same lakeshore 3fl, Tormach 3fl's both with 45° helix's in TiCN and CrN. The Tormach 3fl in TiCN has been the fastest for me, it's what I'm using in this video, I've done this same opp, it's 0.4DOC, 0.075WOC, @103IPM .

https://www.dropbox.com/s/aii6dek7pa...04150.mp4?dl=0

I'm pretty happy with this half inch end mill but I'm still looking for something better, still trying to decide if in going to go with a corn cob or an insert cutter. .

Sent from my SM-G900V using Tapatalk

[cobrakai]

Impressive video. Sort of off-topic - Question... it looks like you spiral in, and then use some high speed path to ultimately go into a big circular spiral. When the initial circle is small, isn't the cutter effectively engaging more material, creating a greater chip load? What spiral plunge parameters do you use?

2.8 MRR is nearly the quoted maximum I've read here on the forum. I look forward to a review if you try a corncob cutter.

[tbev]

Thanks @cobrakai ! I've been going a little soft on the ramping. I'm using a f360 2D Adaptive op, it's ramping in at 42ipm, goes down to about 0.4doc than starts opening. The ramp is at the same RPM, it's 4 degrees, and I'm not sure about the rest of the parameters, I'll post them tomorrow. I'm not sure how consist the chipload is throughout the two parts but I know add I have it currently it's a little less aggressive in the ramp than it is during the rest of the time. Notice the bird's nest. That's something I need to play with a bit I've just been spending most of the time getting the mrr up on the rest of the op. .

I'm really quite happy with how well it's going but I want to get something a little better, in half inch, thigh what I really need is a 3/16in cutter as well. I have over an hour of cutting with a 3/16in em in this fixture so that's where I can really cut some time down. I'm currently running a Destiny Viper faster than an M.A. Ford, Keyocera and a couple other 3/16 end mills I've tried. If anyone has a kick ass 3/16 end mill with 0.75in loc I'd love to hear about that too! I'll share everything I find out as well.

Sent from my SM-G900V using Tapatalk

[AUSTINMACHINING]

I found recently I can get the same MRR with a 1/4" end mill as I can with a 1/2" as long as my geometry suits the DOC. These machines are limited by horsepower, and at 1hp, I can get 3 cubic inches per min in 6061 with a 1/4" end mill and they are a lot cheaper than a 1:2". This is running 6000rpm, .6"DOC,.05" WOC and 100 ipm. End mill is YG1CUTTINGTOOLS alupower 3 flute.







https://m.youtube.com/watch?v=dPXj9FKwFXYm

[tbev]

That's at 0.6 or 0.06in DOC with that quarter inch cutter?

I'm all for cheaper bits, at this point actually I'm willing to pay anything if it will remove material faster, really..for production's sake. I can see that a 0.25in bit wouldn't bog the machine down but I am getting to the max cutting ipm on my machine as well, it's 110ipm I think, and I'm running the half inch bit at 100-103ipm so the only real place to go from here is more WOC or DOC, or both, which I'm having a hard time grasping a 0.25 or 0.375 bit will take more of than a 0.5in bit .

I do agree the Tormach 1100 is being pushed pretty hard and probably can't even run a half inch bit optimally, but I'm not sold on more MMR from a 3/8 or 1/4in end mill at any feed/speed/DOC/WOC combo than a 1/2in end mill.
I would live to be proven wrong, like you said, they are cheaper and for my application using a smaller but will leave less rest material to remove so it would be fantastic if it were the case.

Here's a shout if the parts I'm making with this recipe of 1/2in roughing and 3/16 finishing.

[AUSTINMACHINING]

That's at 0.6 or 0.06in DOC with that quarter inch cutter?

I'm all for cheaper bits, at this point actually I'm willing to pay anything if it will remove material faster, really..for production's sake. I can see that a 0.25in bit wouldn't bog the machine down but I am getting to the max cutting ipm on my machine as well, it's 110ipm I think, and I'm running the half inch bit at 100-103ipm so the only real place to go from here is more WOC or DOC, or both, which I'm having a hard time grasping a 0.25 or 0.375 bit will take more of than a 0.5in bit .

I do agree the Tormach 1100 is being pushed pretty hard and probably can't even run a half inch bit optimally, but I'm not sold on more MMR from a 3/8 or 1/4in end mill at any feed/speed/DOC/WOC combo than a 1/2in end mill.
I would live to be proven wrong, like you said, they are cheaper and for my application using a smaller but will leave less rest material to remove so it would be fantastic if it were the case.

Here's a shout if the parts I'm making with this recipe of 1/2in roughing and 3/16 finishing.

That is .6" deep. If you watch the video, you can see the length of the chips. My point was not that you can remove more than a half inch end mill, but that you are limited in horsepower, so it doesn't matter what size the end mill, you are typically not going to get more than 3 cubic inches per horsepower in aluminum. You can with a specialty cutter like the shear hog. I have one, but it can't get into small corners etc. If I were going to try a new endmill that may do better than 3 cu", I would look at the destiny tool diamondback. It is made specifically for roughing aluminum, and comes in any diamter

[tbev]

Cool, I was hoping you were going to say that. I certainly wound love to use the smaller bit, to get into the corners more, and leave less for this sorry ass 3/16 bit to have to deal with. Do you think I can hit 2.8 or 3 ci with the 3/8in diamondback ?

Sent from my SM-G900V using Tapatalk

[SCzEngrgGroup]

I found recently I can get the same MRR with a 1/4" end mill as I can with a 1/2" as long as my geometry suits the DOC. These machines are limited by horsepower, and at 1hp, I can get 3 cubic inches per min in 6061 with a 1/4" end mill and they are a lot cheaper than a 1:2". This is running 6000rpm, .6"DOC,.05" WOC and 100 ipm. End mill is YG1CUTTINGTOOLS alupower 3 flute.

A 1/4" endmill will certainly have FAR more flex than a 1/2" endmill (roughly 1/4 the stiffness), especially at that depth. If cheap is your goal, do what I do - use HSS endmills. I do most of my roughing at 6000 RPM, up to 150 IPM with 1/2" HSS endmills in 6061. They only cost about $12 each, and with proper toolpaths, last a looooong time, even running maximum MRR. When a tool gets too tired to use for final finishing, I delegate it to roughing duty, to get even more life out of it. On low HP machines, carbide makes sense mostly on smaller tools, to limit flex.

Regards,
Ray L.

[tbev]

I'm not going for cheap tho, it's a nice byproduct if it will move as much material but I'm looking for the most removal. If I can remove as much as fast with a 3/8in em as I am with a 1/2in em than I'm all in, I'm just a bit skeptical. I will certainly pay more for more removal, however I get it.

Sent from my SM-G900V using Tapatalk

[brianbonedoc]

Tom - if you want to increase the speed of the machine you can modify the .ini file pretty easily.

I am not sure how fast the 1100 can go but my novakon pulsar I have cranked up to 300ipm per axis! I even had it running 420 ipm but would occasionally miss steps.
Combined axis movement on the rapids are over 500ipm.

To find the ini file hit ctl-shift-x i believe. Then type in gnome-panel. This will bring up the desktop.

Open up file explorer and look for the tmc folder and then configs -> tormach_mill

Open up tormach_1100_3.ini and then you see sections like this for each axis. Axis 0=x Axis 1=Y Axis 2=Z and remember the units are per second, so for IPM multiply x60.

[AXIS_0]
TYPE = LINEAR
HOME = 0.000

# Default=110 in/min 1.833/30.0
MAX_VELOCITY = 5
MAX_ACCELERATION = 22

# 20 % higher max-vel and 50% higher maxaccel for backlash comp 7.2/26
STEPGEN_MAX_VEL = 6
STEPGEN_MAXACCEL = 26
---------

Also to set max combined axis velocity it's this section:

[TRAJ]
AXES = 4
COORDINATES = X Y Z A
LINEAR_UNITS = inch
ANGULAR_UNITS = degree
DEFAULT_VELOCITY = 1.5
MAX_VELOCITY = 7.5

---------


Don't worry you can always change things back if you hear the steppers stall/squeal a bit.

[tbev]

Tom - if you want to increase the speed of the machine you can modify the .ini file pretty easily.

I am not sure how fast the 1100 can go but my novakon pulsar I have cranked up to 300ipm per axis! I even had it running 420 ipm but would occasionally miss steps.
Combined axis movement on the rapids are over 500ipm.

To find the ini file hit ctl-shift-x i believe. Then type in gnome-panel. This will bring up the desktop.

Open up file explorer and look for the tmc folder and then configs -> tormach_mill

Open up tormach_1100_3.ini and then you see sections like this for each axis. Axis 0=x Axis 1=Y Axis 2=Z and remember the units are per second, so for IPM multiply x60.

[AXIS_0]
TYPE = LINEAR
HOME = 0.000

# Default=110 in/min 1.833/30.0
MAX_VELOCITY = 5
MAX_ACCELERATION = 22

# 20 % higher max-vel and 50% higher maxaccel for backlash comp 7.2/26
STEPGEN_MAX_VEL = 6
STEPGEN_MAXACCEL = 26
---------

Also to set max combined axis velocity it's this section:

[TRAJ]
AXES = 4
COORDINATES = X Y Z A
LINEAR_UNITS = inch
ANGULAR_UNITS = degree
DEFAULT_VELOCITY = 1.5
MAX_VELOCITY = 7.5

---------


Don't worry you can always change things back if you hear the steppers stall/squeal a bit.

Oh God, you just got me all excited! I'm pretty much got all my step/depts dialed in to be perfect under the 110 limit. I think there are a few ops I could use an extra 10-20% tho. I'm gonna check it out, I may be chasing you down with more questions soon!

Sent from my SM-G900V using Tapatalk