[tbev]

Is there an easy way to get more RPM?

Sent from my SM-G900V using Tapatalk

[cobrakai]

I got to looking at those YG-1 tools. What about their "speed freak"? Looks kinda like a corncob but not. 1/2" 3Flute 1-1/4"LOC T15 TiCN Coated Aluminum Rougher Speed Freek YG-1 #66515PC | eBay

[IMT]

A 1/4" endmill will certainly have FAR more flex than a 1/2" endmill (roughly 1/4 the stiffness), especially at that depth. ...

Actually a 1/2" EM will be around 16X stiffer than a 1/4", with the same stick out and similar geometry and material. Stiffness is dependent on the section modulus, which for a circle changes with Diameter^4.

[tbev]

So I've invested the stepover to 0.85in, kept the DOC at 0.400 and set the feed at 100ipm and moved from the 45,° helix 1/2in 3fl to a 3/8in INCO Streaker, same helix, 3fl. I'm getting the op done a little faster, the mmr is a bit higher and it's leaving much less material to remove with the following finishing operations. This has allowed me to run the finishing ops way faster and reduce the total run time by 30%!!! I'm removing material significantly faster with the 3/8 than I ever have with a half. It's also wort noting I've been told many times that a corn cob won't get close because they require more hp.

The best half inch rougher for the 110p it's a 3/8. Hope this helps someone out, I'm very happy.

Here's a quick video:

https://www.dropbox.com/s/8epo9dj3jy...01411.mp4?dl=0

Sent from my SM-G900V using Tapatalk

[wtopace]

I've been told many times that a corn cob won't get close because they require more hp.

The best half inch rougher for the 110p it's a 3/8. Hope this helps someone out, I'm very happy.

Really glad you got it settled!! Congrats on the awesome MRR. That's basically where I landed, corn cobs require massive machine stiffness and HP to be effective, grab a real VMC and you're good to go, but not on the Tormach. I have found that I can blast through 1018 or A36 steel with a 3/8 variable helix endmill waaaay faster (and quieter!) than a standard 30 degree helix or corn cob.

I would equate modern geometries in endmills to modern coatings for lathe inserts - game changers in the industry.

Next step for you - a VMC with a real spindle =) Hopefully less sad IG posts also.... #cryforthehaimer

[cobrakai]

So I've invested the stepover to 0.85in, kept the DOC at 0.400 and set the feed at 100ipm and moved from the 45,° helix 1/2in 3fl to a 3/8in INCO Streaker, same helix, 3fl. I'm getting the op done a little faster, the mmr is a bit higher and it's leaving much less material to remove with the following finishing operations. This has allowed me to run the finishing ops way faster and reduce the total run time by 30%!!! I'm removing material significantly faster with the 3/8 than I ever have with a half. It's also wort noting I've been told many times that a corn cob won't get close because they require more hp.

The best half inch rougher for the 110p it's a 3/8. Hope this helps someone out, I'm very happy.

Here's a quick video:

https://www.dropbox.com/s/8epo9dj3jy...01411.mp4?dl=0

Sent from my SM-G900V using Tapatalk

I'm trying to wrap my head around how the 3/8" is faster. Are you pushing a bigger chip per tooth?

Also how does the 45 degree helix help - does it cause more of a slicing action rather than a shearing action as the cutting edge goes through the aluminum? How does it affect chip evacuation? What about TTS pull out with the high helix? I'm actually needing to buy some tools now so I'd like to go with your recommendation. I also seem to manage to chip the tips of the cutting teeth accidentally - are you using a tiny corner radius, or sharp corner?

[tbev]

Thanks buddy @wtopace ! I'm really close to jumping on a new machine, I'm just being cautious and I'm not sure what kind of parts I'll be making with or just yet. Man I really want something with 1000+ipm rapids..

Sent from my SM-G900V using Tapatalk

[tbev]

I'm trying to wrap my head around how the 3/8" is faster. Are you pushing a bigger chip per tooth?

Also how does the 45 degree helix help - does it cause more of a slicing action rather than a shearing action as the cutting edge goes through the aluminum? How does it affect chip evacuation? What about TTS pull out with the high helix? I'm actually needing to buy some tools now so I'd like to go with your recommendation. I also seem to manage to chip the tips of the cutting teeth accidentally - are you using a tiny corner radius, or sharp corner?

I generally need as little of a radius as possible, this IMCO STREAKER is a 0.01rad I think. You can get more of a rad if you want from western tool. It's the same 45,° helix actually, I'm taking more stepover than I was with the half inch bit, bigger chips for sure and feeding it just as fast. Because it goes so much farther into the corners I have way less material to remove with the following 3/16 bit and thus I can push that but way faster and save a ton of time. I'd definitely recommend IMCO, the streaker series, Destiny, and the Tormach end mills, but the half inch but isn't worth using anymore IMO, unless for some reason it was called for. Cheaper and faster, WIN WIN.

https://www.dropbox.com/s/lh88yyrhew...14532.mp4?dl=0

[cobrakai]

What do you finish with?

Crazy you can hear the machine straining lol. Did you mean you're taking a 0.085" stepover btw? It would be nice to see the actual cutting instead of a pool of coolant, but then it wouldn't work as well. What coolant are you using?

[tbev]

Yeah sorry, 85tho stepover, 0.085in. 0.400DOC four hundred thousandths deep. 100-103ipm..

It definitely boggs down a bit, but it stays consistent once it gets bogged down, it's fine. I'm in about the 150th part bogging down like that and haven't had any trouble. Tormach techs say as long as it's not stalling or breaking the cutter it's fine.
I'm using Qualichem, 291, which is for titanium but it works just as good if not better than their aluminum juice 251C, I use that too just but atm.. His keep that coolant going tho, the chips are huge and plentiful, so I gotta get them out of there. Chips are much bigger in size than the child the 3fl 1/2in end mill makes.



Sent from my SM-G900V using Tapatalk

[cobrakai]

Good stuff. I'm glad you found success.

Looks like good coolant. I switched from KoolMist synthetic flood to 585XT semisynthetic flood and it was night and day. Tools last 10x longer, mirror like finish. Last time I ever use a synthetic.

[tbev]

Agreed, I've been really happy with Qualichem, it smells nice and feels ok on your skin, I have a lot of pressure and I get wet sometimes. But it's been fantastic on titanium and aluminum.

Sent from my SM-G900V using Tapatalk

[cobrakai]

So I actually have a 3/8" end mill I'm going to try with your parameters. It's a 38 degree helix 3FL carbide uncoated. Only thing is its a 1.75" flute length (long version) so flexy harmonics might be killer.

[tbev]

I'd choke up as much as I can and start slower. I'm pushing it pretty hard I would start with fifty tho WOC with that much more stickout . Mines a 45° helix so that should rough better in that regard but the length is gonna kill ya. I pulled two pieces of stock out of my fixture. Grabbed they were not held in "optimally" they were less than perfectly held in place but I ran two pretty aggressive ops on the parts first and they held on but when I got to my roughing opp with the 3/8 em they both pulled out.


Sent from my SM-G900V using Tapatalk

[AUSTINMACHINING]

3.4 cu. In / min.. nicely done.!. I'm alway pushing the ragged edge of horsepower, so if I'm doing shallow cuts, I,m less likely to stall the spindle when using a smaller endmill. If I need the stiffness for deep cuts I'll go to a 1/2 inch. For roughing operations tool flex doesn't concern me (as long as it doesn't break :-).