Something I thought I would share.

[crazy^millman]

Sorry ITAR plant so cannot share pics, but cutting some manifolds on a Mori NH-5000. On the 2nd op using a 1/2 3 Flute description of holder and part number of endmill below. Stick out is 1.75.

 

3 FLUTE CARBIDE ROUGHER   CAT 50 LYNDEX CAT50-C1-135U HELICAL 29422

 

Machine is running this tool at 450 ipm with Opti-Core using 10% step over and 200% step down. Machine only has 8000rpms on this 50 Taper, but I have to say I love seeing pop corn coming off the parts. If you cant get excited watching that what will get you excited to be a machinist.

[Pitka_Guru]

Thats pretty sick!  It still amazes me every time I see high feed and speeds cutting steel like it's MDF. What brand and model endmill are you using and what is the material?

[crazy^millman]

On the 2nd op using a 1/2 3 Flute description of holder and part number of endmill below. Stick out is 1.75.

 

3 FLUTE CARBIDE ROUGHER

 

Thats pretty sick!  It still amazes me every time I see high feed and speeds cutting steel like it's MDF. What brand and model endmill are you using and what is the material?

 

HELICAL 29422

 

HTH

[reidmachine]

Cool stuff Ron, Thanks for passing the info along!

Still running my 7.5 hp minimill at 120ipm in 4340, 1/2 dia, 5 flute SGS, 1.0 deep, I suppose if I dropped from 20% stepover to 10% stepover, I could probably get it to run over 200.

Whaddya think?

[Hertz]

Yes Reid. Drop 8-10% and you could really crank the xxxx out of the feed.

[reidmachine]

 had it running over 180 before, machine got real jerky, 2005 vintage.

I'm actually jealous of Ron, 400 just has a good ring to it.

[crazy^millman]

Reid it is a blast to go into companies and help them change. I still remember my day at your place and it was good to spend the day working elbow to elbow with you and your guys. I tried the rougher after seeing the results you were getting with it. Much nicer chip than those long stringy things coming off 1.5 long. These are about 1/4 long .018 thick and they look like confetti coming off the material. The customer has another machine there with 14k spindle. It is a 40 taper, but I will be seeing if I can get 800ipm out of it.  I really think I can make it happen. I am taking parts that normally would have been 18 to 24 hours and getting them done in 3-1/2 hours, with wire holes, cross holes and deburred as much as I can get to. Those were all being done conventionally, but not anymore. They look like your work coming off the machine and these are manifolds for aircraft. I love kicking parts out like that. I love it when a whole organization takes notice of your effort. I am blessed to share and thankful I have the ability to do so.

 

Yes the Smaller the step over the harder you can push the endmill. I am back feeding at 750ipm and really considering bumping that up to 1500ipm. I think the machine can handle it. Fun I tell you just having a good time doing something I am meant to do and that is help others and impart anything I can on those willing to listen. I stop by and say hey another day, but right now I am buried with work and really happy to have it. Make up for the feed by keeping a smaller Depth and higher step over. You have already found the sweet spot for your machine, but on the new one you might try it over there.

[Pitka_Guru]

Ron, another Brand question lol, I'm assuming these companies where you are running 600+ ipm feeds have Makino's or similar high quality high speed machines?

[crazy^millman]

Mori Seiki and I was surprised as anyone, but I am going to push and push and see what it will take. Will not know until you try. Worst I do is break and end mill. When I do I will back it off 10% and call it blessed to run.

 

Anyone can do what I do. I was telling a VP all it takes is some umption and gumption. The umption is the thought or willingness to want to try and gumption is the putting that into actions then seeing it through to get it done. Many people talk a good talk, how many are willing to walk the walk and just keep walking it? Not easy not making it out to be a cake walk, but little hard work, a little effort and anyone can do what I do. Thing is some many think they are already there and just don't realize their not. I learn something everyday in this profession and I mean just about everyday. That is what make it fun.

[Bob W.]

Just out of curiosity, why only three flutes? I am generally trying to get the most flutes I can because I calculate feed based on FPT and more flutes = higher feed rate. 450 IPM is nothing to sneeze at for sure, I haven't got anywhere near that and I hardly every break end mills. Maybe time to push a little harder and break a few. That is money well spent finding the limits.

[crazy^millman]

Cutting Alum and with that width of cut I could probably go up to a 5 flute, but problem is no one coats them for Alum they are all coated for Steel or Heat treated steel and Alum will stick to certain coatings and load up the tool. I wish Helical would offer the 5 flutes with the Z plus coating. That bigger core kicks butt. I am finishing the parts with a 5 flute 3/4 with .06R that has a 2.75 LOC and doing that in one pass and the part looks like glass when done. I am not running them like I am the rougher. The other thing is those long stringy chips using the Rougher style like Reid pointed out to me makes nice manageable chips. I learn something all the time why I love doing this.

 

Other thing would be I am not sure this machine would handle the feed needed to push a 5 flute to the sweet spot to remove the material needed. I am thinking about a 30k spindle with 2000 ipm feed rates would be just run to watch.

[Bob W.]

I don't recall what material you were cutting? Steel or aluminum? Alloy? The step over makes me think steel but three flutes and 450 ipm makes me think aluminum. If it is aluminum, why not run a 25-30% step over? Too much load on the tool?

[brandon b]

Hey ron have you done any of this high feed rate on a fadal vmc. Thats all our company has. Fastest ive ran an opti rough toolpath was 120 ipm and it looks like the machine is going to self destruct anytime...plus the boss freaked out when i was roughing aluminum at 80 ipm. With a 200 ipm back feed rate. Said i was destrying his machines

[neurosis]

I don't recall what material you were cutting? Steel or aluminum? Alloy? The step over makes me think steel but three flutes and 450 ipm makes me think aluminum. If it is aluminum, why not run a 25-30% step over? Too much load on the tool?

 

I agree.  Its not quite as fun to watch but your CIM would go up quite a bit.

 

We have a job that we use a 1/2" SGS S-Carb on.  30% step over,  240% axial (1.2) @ 240 ipm. This is on a Mori NH4000 40 taper machine. Our CIM is 43.2. It looks like Ron is running right around 22.5 CIM? Our limiting factor at this point is spindle load.

 

It certainly sounds like it might be fun to watch though. 

[Bob W.]

For 95% of my roughing I will run a 1/2" MA Ford 134 series at 30% step over, 200% LOC, and 400 ipm. This is at 14000 rpm so the chip load is pretty low. I have run these as high as 800 ipm but at those feeds they tend to break and the down time to replace the tool outweighs any time advantage from running faster (usually the machine is unattended so it might sit for a while). At the 400 ipm they never break.

[Bob W.]

Hey ron have you done any of this high feed rate on a fadal vmc. Thats all our company has. Fastest ive ran an opti rough toolpath was 120 ipm and it looks like the machine is going to self destruct anytime...plus the boss freaked out when i was roughing aluminum at 80 ipm. With a 200 ipm back feed rate. Said i was destrying his machines

How does he compete? I rough hardened steel (RC45) at triple that feed rate...

[MIL-TFP-41]

Crazy....5 flutes for alum? you got it....

 

http://benchmarkcarbide.com/catalog/products/55050020.html

 

Benchmark does make some nice stuff.

[brandon b]

How does he compete? I rough hardened steel (RC45) at triple that feed rate...

i have no idea. We dont do any big runs ,just a few pcs every month. Lean manufacturing...as i guy on the shop floor i hate it, sucks having to setup a job and tear it down and then setup again 2 weeks later. Nothing is repeatable.just slap a vise where it fits and indicate fixtures flat on machine tables that arnt flat. One of our 80 inch tables is out 50 thou from one end to the other.

[Joe788]

I think there are some situations where dynamic and opti paths work awesome in aluminum with the big DOC and small axial cut, and I use them both pretty frequently - but if you've got a medium sized part with a lot of bulk to come off - a 2 inch Mitsubishi AXD cutter using an optirough path with a large stepover, and small step down,  will move a lot more material a lot faster than an endmill.

[neurosis]

It would be nice if there was a dynamic strategy specifically for large radial and small axial cutting. One of the things that I miss with Volumill, was that rather than making 10,000 tiny loops in tight areas, it had the option of picking up and channeling straight through the tight areas which saved a lot of time. Dynamic does have the zig zag now but I am not a big fan of conventional cutting (probably just being a sissy).  With the light axial cut there is no reason not to be able to channel straight through.

 

The old core roughing HSS paths suck so I rarely use them.

[Newbeeee™]

For 95% of my roughing I will run a 1/2" MA Ford 134 series at 30% step over, 200% LOC, and 400 ipm. This is at 14000 rpm so the chip load is pretty low. I have run these as high as 800 ipm but at those feeds they tend to break and the down time to replace the tool outweighs any time advantage from running faster (usually the machine is unattended so it might sit for a while). At the 400 ipm they never break.

We use the 14mm diameter for all of our work, and the 12mm for the parts that are a bit smaller.

We standardised on this for all machines (both 40 and 30 tapers).

The 40 tapers run the 16mm diameters well, but the 30 tapers are too noisy for the 16mm.

On the 40 tapers we'll run at 100% LOC and 30% stepover and 10krpm and 7.5 m/min (300 ipm) and I thought we were doing well...

As they say, every day's a school day

[Newbeeee™]

1.  One of the things that I miss with Volumill, was that rather than making 10,000 tiny loops in tight areas, it had the option of picking up and channeling straight through the tight areas which saved a lot of time.

 

2.  The old core roughing HSS paths suck so I rarely use them.

1.  This would rock! Great enhancement, and must suck for you since you had this feature a couple of years ago now and have since lost it...

 

2. 100% agree.

[Bob W.]

I really liked how Volumill would allow a ramping contour through the tight areas. Say I am roughing a peanut shaped cavity with a .25" cutter and the narrow region of the cavity is .275" wide, there is really no practical way to get through there with troichoidal (sp?) motion. Volumill would adopt a high feed approach where the cutter would be taking much smaller depth cuts to clear that region. It was really slick and saved from either having to piece together a few more toolpaths to get it done or a rest-milling toolpath with a much smaller cutter. I have no complaints regarding Mastercam's 2D HST toolpaths but that would be a slick enhancement.

[Newbeeee™]

So being an idiot here, I 'thought' the reason why volumill add-on was dropped was because mastercam's new HS toolpaths could internally do what volumill could do??? 

Not knowing volumill could do what you said, this to me, seems a big thing? So is mastercam working on implementing this strategy because this would be awesome (over used word I know but it would be )???

I see they sell a stand alone volumill nexion http://www.volumill.com/content/learn-more-about-volumill-nexion