What's new
What's new
By:
Advanced search…

reality check... how fast/hard are you machining aluminum lately?

lowCountryCamo

lowCountryCamo

Stainless
Joined
Jan 1, 2012
Location
Savannah, Georgia, USA
I program at an aerospace job shop. We make mostly structural parts for corporate aircraft. I program with Mastercam and rough using "dynamic" or side engagement milling. If possible I go full depth. I use mostly 3/8 and 1/2 endmills with a corner radius cutting 7000 aluminum. Machines vary from horizontals, large verticals, 5x vertical, to a little Haas. I feel like I might be under feeding and stepping for fear of breaking tools and scrapping parts. Generally I feed 80-130 ipm .07-.12 radial steps. I use each machines max rpm on Al. I know this is a general question that may be hard to answer.

Thanks.

Steve A
 
Is full depth 3/8" or 3/4" or 2"? It makes a difference.

But unless your mills only have 4000 rpm or something you can bump the feed up rather a lot. My standard rough with a 1/2 in aluminum is .1" stepover and 250ipm at 16000rpm. That's with a 7hp 30 taper. You can probably push harder if you have something with more grunt and rigidity.
 
IMO you need to approach each machine differently and program to their strengths. The place I retired from did lots of trial cutting when a new machine came in to establish a bunch of best cutting conditions for that machine. Then programming would use those cutting conditions as much as possible from then on. The testing evolved to the point of buying a tap test setup. Then we could narrow in on the spindle and tool assembly dynamic more quickly. A major upside was that tool breakage happened in the testing phase. Once stable cut conditions were developed and implemented tool breakage in a production part was a rare occurrence.
 
Too many machinists focus on high RPM and high IPM numbers when roughing....especially that guy with all the youtube videos that screems BOOOOOM all the time.
Ya great, you're cutting at a super high rpm/ipm but you're making a ton of super light cuts which results in a lot of repositioning moves (not making chips) and cutting in an RPM range that does not have a lot of tourque. Which all leads to either low MRR (metal removal rate) or high cycle times. When roughing the only numbers you should be concerned about is MRR and to take it one step further MRR that includes the time needed for cutter repositioning (cycle time).
Use your load meters to see how close to max you are pushing the machine. Experiment with different RPM ranges to see if you can increase the MRR. You may find running a lower RPM gets you the additional HP/Torque to take a bigger cut....bigger cuts mean less repositioningmoves

Mastercam Dynamic Motion - Power vs. Speed Cutting - YouTube

Theres an example of a high MRR but cycle time is lower with the part being machined at a lower MRR, just due to the lack if repositioning moves.
 
With 1/2” and 3/8” Diamondbacks:

16,000 RPM
288 - 384 IPM
25-40% radial DOC (aka engagement)
Up to 2.5xD axial DOC

Yes, backfeed loops waste time, but your CAM should let you backfeed at a much higher IPM, or even backfeed at rapids speed. That video you linked uses painfully slow backfeed speed.

I should also point out that IME at least, optimizing the roughing isn’t terribly compelling since I usually spend way more time on finish passes, remachining with small endmills, chamfering, and other detail work.

Regards.

Mike
 
Finegrain said:
....I should also point out that IME at least, optimizing the roughing isn’t terribly compelling since I usually spend way more time on finish passes, remachining with small endmills, chamfering, and other detail work.
Click to expand...

+1^

On most jobs it is way more important to have the programmer look for ways to improve the finishing operations than to try to eke out a bit higher roughing MRR.
 
Finegrain said:
With 1/2” and 3/8” Diamondbacks:

16,000 RPM
288 - 384 IPM
25-40% radial DOC (aka engagement)
Up to 2.5xD axial DOC

Yes, backfeed loops waste time, but your CAM should let you backfeed at a much higher IPM, or even backfeed at rapids speed. That video you linked uses painfully slow backfeed speed.

I should also point out that IME at least, optimizing the roughing isn’t terribly compelling since I usually spend way more time on finish passes, remachining with small endmills, chamfering, and other detail work.

Regards.

Mike
Click to expand...

Maybe this video is a better comparison then...
Mastercam Dynamic Milling - YouTube
There are 4 videos in there, the most efficient is again the power cutting technique.

Yes, roughing is only one aspect of the process which is what I thought OP was focusing on so I replied with that in mind. Finishing is a whole other ball game...2D vs 3D...bull vs ball vs barrel...knowing the Ra required for the surface and how that relates to feedrate.
 
expensive part where boss gets upset over scrap parts you machine different. for many even a 1% scrap rate is totally unacceptable.
.
usually i look at load meter and whether i can hold a part and not have it move in vise or fixture.
 
Matt@RFR said:
All four videos show a HSM toolpath with different parameters. What is your argument?
Click to expand...

The bottom right video shows a very high 75% stepover, which is more of a traditional toolpath. I'm amazed the endmill survived that! It's more of a testimonial to the endmill than to the toolpath. I have to wonder about tool life with such a high engagement.

Regards.

Mike
 
goooose said:
Too many machinists focus on high RPM and high IPM numbers when roughing....especially that guy with all the youtube videos that screems BOOOOOM all the time.
Ya great, you're cutting at a super high rpm/ipm but you're making a ton of super light cuts which results in a lot of repositioning moves (not making chips) and cutting in an RPM range that does not have a lot of tourque. Which all leads to either low MRR (metal removal rate) or high cycle times. When roughing the only numbers you should be concerned about is MRR and to take it one step further MRR that includes the time needed for cutter repositioning (cycle time).
Use your load meters to see how close to max you are pushing the machine. Experiment with different RPM ranges to see if you can increase the MRR. You may find running a lower RPM gets you the additional HP/Torque to take a bigger cut....bigger cuts mean less repositioningmoves

Mastercam Dynamic Motion - Power vs. Speed Cutting - YouTube

Theres an example of a high MRR but cycle time is lower with the part being machined at a lower MRR, just due to the lack if repositioning moves.
Click to expand...

It's VERY situational.
Right now I'm cutting a 1,000pc job of 6061 alum with a 1/2" 3 flute Destiny Diamondback.
Ramping in 1.200" deep,and cutting a 3"x 4" pocket (each corner has a form,not just a square pocket) at 15,000 rpm and 460IPM with a .100" stepover. Less than 30 seconds per pocket. You can't beat that with conventional toolpaths.
The main reason for HSM paths is because you don't need to torque the clamping down so much as when you're hogging. Thus preventing part distortion.
I had to go with a Destiny Diamondback endmill because a regular 3 flute makes chips too big and would clog up the augers. The chipreaker is a dream come true for the volume of chips coming off these parts.
This is done on an Okuma Genos M560V with 30HP.
Technically 55 cubic inch MRR
 
lowCountryCamo said:
I program at an aerospace job shop. We make mostly structural parts for corporate aircraft. I program with Mastercam and rough using "dynamic" or side engagement milling. If possible I go full depth. I use mostly 3/8 and 1/2 endmills with a corner radius cutting 7000 aluminum. Machines vary from horizontals, large verticals, 5x vertical, to a little Haas. I feel like I might be under feeding and stepping for fear of breaking tools and scrapping parts. Generally I feed 80-130 ipm .07-.12 radial steps. I use each machines max rpm on Al. I know this is a general question that may be hard to answer.

Thanks.

Steve A
Click to expand...

I spend a lot of time roughing aluminum, both 6061 and 7075. My machines range from 6000 rpm to 12000 rpm. I use almost the same parameters as you do with a 1/2" EM. 6000 RPM, 1 inch depth of cut, 60 IPM, and .1 radial step. At 12,000 RPM, the IPM goes up to 120 IPM. In aluminum, I almost never go lower than 20% (.1") radial step over, but will go much higher if the cut must be shallower.

I can push the machines harder, but I feel that I get diminishing returns in the form of increased scrap rate, wear and tear on the machines, fixture and cutters, and it requires a higher priced cutting tool. The conditions that you are using are safe and sane for a consistent process.

I feel that there is better return on investment on optimizing cutter paths and parameters (arc filter, back feed rate etc) than by pushing my machines as hard as they will go.
 
G00 Proto said:
I spend a lot of time roughing aluminum, both 6061 and 7075. My machines range from 6000 rpm to 12000 rpm. I use almost the same parameters as you do with a 1/2" EM. 6000 RPM, 1 inch depth of cut, 60 IPM, and .1 radial step. At 12,000 RPM, the IPM goes up to 120 IPM. In aluminum, I almost never go lower than 20% (.1") radial step over, but will go much higher if the cut must be shallower.
Click to expand...

Not to be private investigator or anything, but, you are running very conservatively assuming you have fairly modern machines. Your 12,000 RPM parameters shown above give 12 in^3 per minute MRR. I'm running 40-60 in^3 per minute on my relatively lightweight 30-taper Brother, every day. I have essentially 0 scrap rate due to running too hard. About the only time scrap happens is when I make a programming mistake. Higher priced cutting tools? Yes, but they can pay for themselves within the first day of high-efficiency cutting, and then they last a long time after that. Rough guess is I can put a couple 1000 # of chips into the bin with a single Destiny Diamondback. Actually I have no idea what the wear life of a Diamondback is, as they usually suffer some other, more abrupt fate (usually programming error) before they wear out.

I will grant you that if you have a 20-year old machine that wasn't designed for high feed rates, you are probably asking too much. But, the OP says he works in an "aerospace shop" so I can only assume they have decent machines.

Regards.

Mike
 
on a old machine isnt it better to use a roughing corn cob end mill for roughing ?? smaller chips that wash down to chip conveyor with coolant ??
.
they even sell carbide roughing end mills
 
barbter said:
+1

Regarding the Ops questions:-
BT30 (Robodrill)
14mm MA Ford 134 or Garr Hogmill 3 flute equivalent
DOC 150% Max
Stepover 30"
Toolpath Rad 3mm
Speed 10Krpm
Feed F3500

BT30 Face and Taper machines
14mm MA Ford 134 or Garr Hogmill 3 flute equivalent
DOC 150% Max
Stepover 30"
Toolpath Rad 3mm
Speed 10Krpm
Feed F5000

BT40
14mm MA Ford 134 or Garr Hogmill 3 flute equivalent
DOC 150% Max
Stepover 30"
Toolpath Rad 3mm
Speed 10Krpm
Feed F7500

Depending upon your machines, controls, MTB implementation of the parameters, and highspeed lookahead functions, you may have to fine tune your acc/dec on the servos or those feeds could either be really slow, or knock your thrust bearings out and shake the machine to pieces.
Click to expand...
.
how round a circle you get at those feed rates ?
 
Comparing your shops cutting conditions to youtube videos is a little sketchy. I am guilty of it as well. The last time I was cutting aluminum was back when I was on our Fidia. I don't do allot of aluminum cutting so I was going at The Helical endmill recommendations, which seemed a little conservative, I cranked it up to something more realistic and was quite happy with the results, until I was done and realized that the entire time I was spinning the HSK holder in the spindle taper the entire time. You see, the Fidia spindle does not use the drive lug. I sure got done fast, but I also had to get a new holder, not to mention the time it took inspecting the spindle taper that was luckily alright. There becomes a question of how fast can you go verses how fast should you go and at what expense.
 
DMF_TomB said:
.
how round a circle you get at those feed rates ?
Click to expand...

At feeds of 3000, 5000, 7500 mm/min I would imagine a robodrill or any properly tuned machines will be less than 10 microns (that isn't really all that fast), but it is all going to depend on the circle sizes, anything proportioned properly (cutter<25% of hole), will likely be even better than that, as the acceleration won't be tool bad, with smaller holes and cutters obviously you won't be able to travel that fast accurately as there will be too much acceleration, but properly setup AICC will slow it down.

When I get the time, I'll run a ballbar test and we will see, mind you it won't be under load, but neither really is finishing if done properly.
 
You must log in or register to reply here.

Similar threads

B
How do you deal with revision changes?
Replies
8
Views
2K
MaxPrairie
M
B
Help with speeds and feeds.
Replies
6
Views
2K
Shawnrs
S
B
How would you program milling this bronze part in Fusion 360?
2
Replies
34
Views
6K
implmex
I
Nerdlinger
How Many Parts Are You Getting With Your Parting Tool?
2 3
Replies
54
Views
6K
Ox
Ox
Eric U
Finish issues with tiny boring bar in 4140HT
2
Replies
37
Views
6K
Eric U
Eric U








 

ABOUT PRACTICAL MACHINIST

With more than 10.6 million unique visitors over the last year, Practical Machinist is the most visited site for metalworking professionals. Practical Machinist is the easiest way to learn new techniques, get answers quickly and discuss common challenges with your peers. Register for the world’s largest manufacturing technology forum for free today to stay in the know.

Learn more about us.

STAY CONNECTED

Facebook Instagram YouTube LinkedIn Pinterest Twitter Tiktok

Register Become a forum member. Register today.

Sign Up Sign up for our e-newsletter.

© 2024 Copyright Practicalmachinist.com. All Rights reserved.

Back
Top