[4]

CNC Toolpath Strategies for smaller machines

macardoso

Brass
Registered
Joined
Mar 26, 2018
Messages
631
Just wanted to open a discussion on what people find works well for benchtop class machines for CNC strategies.

I have a 2.5 HP spindle that I would like to take full advantage of. My machine (G0704) does not have the column stiffness to handle tools much larger than 3/8" nor does the 5000rpm max spindle speed allow me to run small tools really fast like a router table would. The sky is the limit when it comes to feedrate and accelerations for me.

I have found that trochoidal toolpaths with full depth of cut engagement seem to work well, but I have always stuck to 15% of cutter diameter stepover in aluminum and roughly .001 to .0015 feed per tooth. This ends up only using <1HP. Specifically for roughing, what strategy would you recommend to take advantage of the remaining spindle power? Would you increase radial engagement for a wider chip or rather increase the chip thickness? Would plunge roughing be worth looking into? I've always wanted to experiment with high feed milling as you can get high material removal with smaller tools at lower spindle speeds.
 

bakrch

H-M Supporter - Gold Member
H-M Supporter - Gold Member ($25)
Joined
Nov 24, 2018
Messages
75
I also find the column to be the limiting factor (PM-25, so similar rigidity). I suppose if I took out the vises and put mitee-bite clamps on a fixture plate this could be optimized, but not quite given up on the vises while cutting at mid-Z-travel yet.

Stock 1hp/2500 RPM motor here and my roughing strategy is 1/2" 3 flute end mill 1.25 LOC (SC YG1 w/ 45 deg helix), .005 IPT, .62 axial, .025 radial (5% stepover). Triple the radial with a 1/4" axial cut and feed/speeds the same. Could probably push it harder, but this has been fairly reliable and with adequate cycle times. I don't need the carbide obviously, but it's what I had available.

Made a bunch of these over the past 8 mos, so tweaking for quite a while now.


 
Last edited:

derf

Brass
Registered
Joined
Oct 3, 2015
Messages
800
I'd go with a 4 flute end mill and a deeper cut.
 

spumco

Active Member
Registered
Joined
Jan 15, 2016
Messages
310
I've got the same floppy colum problem, but I'm working on a column reinforcement (big A-frame column back plate)...

Getting to the point, here's what I'm doing to maximize MRR without chatter

Aluminum
1. 4 flue HSS fine-tooth roughing end mills for aluminum. Better have flood coolant or a good mister, but the 4FL doubles your effective RPM over a 2FL and the chips are very fine - no clogging or nesting. The chips flow out of pockets really well and the tools stay sharp forever. And they are cheap. I use a 1/2" rougher at 5kRPM, 20%, .500"DOC, and 100IPM. For a small mill it's hoggin...

2. Despite using trochoidal toolpaths, I still prefer a slightly shallower DOC and wider WOC. I believe shorter tools and shorter DOC - compared to full flute length - have less leverage on the tool, holder, TTS collet, and ultimately the column. This is relative, of course - try bumping up the WOC to 25 or 30% and taking a shallower cut.

3. I stick with carbide for finishing cuts and small tools just to cut down on tool flex. Column stiffness doesn't really matter with 1/4" and 1/8" end mills (for me).

Steel
1. I use roughing end mills whenever I can, but carbide instead of HSS. I limit my profiling to 3/8" cutters and set the SFM to about 75% of MFGR recommended for better tool life.

2. Air blast for steel and I've noticed my tools stay sharp longer. Sharper = less cutting pressure = more material removal before column bouncing.

3. I have a 5/8 stub bullnose that just plows through steel and Ti. Trick is to use it like a high-feed mill and set the DOC to less than the corner radius. In my case it's a 0.030" corner, so I limit it to 0.025" DOC but with a 85% stepover. There's never any chatter, surface finish looks great and I'm getting a theoretical 2in MRR in mild steel.

All materials
1. Stub length cutters and short tool holders whenever possible.

2. Lower the setup on the table whenever possible. If you can bolt the stock directly to the table - do so. The higher the head is on the column, the more leverage there is against the column twisting or flexing back.

3. Use the high speed machining and chip thinning calculation features in any of the F&S programs. If you don't already have one - GET ONE. I prefer HSMAdvisor. This will tell you if your axis speeds are the limiting factor. You can then start playing mix-n-match based on your max spindle RPM and axis speeds so you don't leave lots of horsepower on the table.

-R
 

ChrisAttebery

Rocket Nerd
Registered
Joined
Jan 11, 2018
Messages
118
I also posted this on cnczone but I'll repost here for those that don't participate there.



I have a G0704 with a 1100W motor on it. I ran it at 4500 rpm for a few years and then bumped it up to 6750 rpm last year. I generally shoot for a MRR of 1.3in/min. I use high quality HSS end mills because they are cheap and these machines don't have the rigidity to use carbide efficiently.

My go to parameters are:
3/8" 2 flute YG-1 aluminum end mill
Speed: 6000 rpm
DOC: .500"
WOC: .05"
Feed: 54 IPM

My general rules for HSM in aluminum are to use full depth, 10-20% WOC, 1-2% feed per tooth. If I need to reduce DOC I increase WOC up to 20%, then I start adding feed. I wish someone made a 3/8" 3 flute in HSS. That would be my next step.

All of this assumes that you have a coolant system of some sort. I use a home brew mist system.

I have used 3/8" 3F carbide end mills in the past. They worked great but cost about 3X what the 3/8" 2F HSS end mills do. I decided that for my needs it wasn't worth the extra expense.

Good luck,


Chris
 

bakrch

H-M Supporter - Gold Member
H-M Supporter - Gold Member ($25)
Joined
Nov 24, 2018
Messages
75
I've got the same floppy colum problem, but I'm working on a column reinforcement (big A-frame column back plate)...

Getting to the point, here's what I'm doing to maximize MRR without chatter

Aluminum
1. 4 flue HSS fine-tooth roughing end mills for aluminum. Better have flood coolant or a good mister, but the 4FL doubles your effective RPM over a 2FL and the chips are very fine - no clogging or nesting. The chips flow out of pockets really well and the tools stay sharp forever. And they are cheap. I use a 1/2" rougher at 5kRPM, 20%, .500"DOC, and 100IPM. For a small mill it's hoggin...

2. Despite using trochoidal toolpaths, I still prefer a slightly shallower DOC and wider WOC. I believe shorter tools and shorter DOC - compared to full flute length - have less leverage on the tool, holder, TTS collet, and ultimately the column. This is relative, of course - try bumping up the WOC to 25 or 30% and taking a shallower cut.

3. I stick with carbide for finishing cuts and small tools just to cut down on tool flex. Column stiffness doesn't really matter with 1/4" and 1/8" end mills (for me).

Steel
1. I use roughing end mills whenever I can, but carbide instead of HSS. I limit my profiling to 3/8" cutters and set the SFM to about 75% of MFGR recommended for better tool life.

2. Air blast for steel and I've noticed my tools stay sharp longer. Sharper = less cutting pressure = more material removal before column bouncing.

3. I have a 5/8 stub bullnose that just plows through steel and Ti. Trick is to use it like a high-feed mill and set the DOC to less than the corner radius. In my case it's a 0.030" corner, so I limit it to 0.025" DOC but with a 85% stepover. There's never any chatter, surface finish looks great and I'm getting a theoretical 2in MRR in mild steel.

All materials
1. Stub length cutters and short tool holders whenever possible.

2. Lower the setup on the table whenever possible. If you can bolt the stock directly to the table - do so. The higher the head is on the column, the more leverage there is against the column twisting or flexing back.

3. Use the high speed machining and chip thinning calculation features in any of the F&S programs. If you don't already have one - GET ONE. I prefer HSMAdvisor. This will tell you if your axis speeds are the limiting factor. You can then start playing mix-n-match based on your max spindle RPM and axis speeds so you don't leave lots of horsepower on the table.

-R
Yeah, I can't even use a TTS holder with my strategy ... pulls it right out. I was roughing with a 3/8" 4fl with larger radial/shallower axial cuts at the same MRR with success, but it also had chatter issues. Haven't gone back to this with the 1/2" 3fl YG1 yet, but I'll be certain to give it a go.

You folks really making me want to replace my motor (and bearings I'm assuming) to get my MRR on par, just have way too many parts to make right now.
 

JimDawson

Global Moderator
Staff member
H-M Platinum Supporter ($50)
Joined
Feb 8, 2014
Messages
7,999
I guess my take on this is to make test cuts at increasing loads to find the machine/tool limits. Then back down a bit and make parts. That's the way we run the Haas, admittedly we are working with a lot more machine, but it's all relative. But I have found using trochoidal cutting on my knee mill I can increase the MRR by quite a bit. But I don't run the machine that hard, normally not more than 60% power, or about 2 HP out of 3.
 

macardoso

Brass
Registered
Joined
Mar 26, 2018
Messages
631
Thanks all! I haven't had a chance to really rip with this new setup but I am excited to. I use YG1 ALU-POWER 3F carbide endmills in aluminum (mirror finish even when cutting dry or minimal coolant). I should be able to monitor spindle load in real time as well, so I'm guessing it will come down to rigidity.

Not trying to set any records here, but I think I can comfortably increase my MMR beyond my current recipe and I think the suggesting above will help do that! Thanks!
 

spumco

Active Member
Registered
Joined
Jan 15, 2016
Messages
310
Regarding TTS pullout - use a torque wrench to tighten your drawbar. 7/16-20 drawbars can take a fairly good amount of torque - I shoot for 25ft-lbs of prelead on my belleville stack. If you're just uding a drawbar with no spring stack (no PDB, in other words), anti-seize the collet taper slightly and the drawbar threads & washer. You may find the holding power has gone up considerably.

Still not a guarantee which is why I'm switching to a BT30 spindle shortly.
 

bakrch

H-M Supporter - Gold Member
H-M Supporter - Gold Member ($25)
Joined
Nov 24, 2018
Messages
75
Regarding TTS pullout - use a torque wrench to tighten your drawbar. 7/16-20 drawbars can take a fairly good amount of torque - I shoot for 25ft-lbs of prelead on my belleville stack. If you're just uding a drawbar with no spring stack (no PDB, in other words), anti-seize the collet taper slightly and the drawbar threads & washer. You may find the holding power has gone up considerably.

Still not a guarantee which is why I'm switching to a BT30 spindle shortly.
Thank you for the anti-seize tip, worked quite well!
 
Last edited:

ChrisAttebery

Rocket Nerd
Registered
Joined
Jan 11, 2018
Messages
118
I was poking around on YG's website and I found a 3 flute HSS roughing end mill for aluminum. The part number is 66305. My local distributor has them for $27.25 each. The 17055 I normally use are $11.65 each. At the moment I don't have any projects where I need to do a lot of roughing. If something comes up I'll try one out and report back.

http://www.yg1usa.com/feature/itemdetail.asp?edpno=66305
 

macardoso

Brass
Registered
Joined
Mar 26, 2018
Messages
631
Nice Find! I'm a fan of 28584 from them. Really does a nice job in aluminum.
 

brayan

Registered
Registered
Joined
Apr 26, 2019
Messages
1
It's a great discussion and will help everyone to learn new things and strategies. Well, there are different components that contribute to an effective machining process in high-speed for mold and die makers. As we have learned a lot on the impact of HSM on CNC machine and cutting tools, spindles, and more importantly controls. We also ignore the fact that high-speed machining impact on tool path and programming techniques. Now machining technologies are evolving and meet the specific needs of new tool path strategies designed to suit the HSM environment.

In HSM environment we can use higher spindle speeds and feed rates for removing materials faster without compromising the part quality. This strategy applied to finish dies and mil modes to net shape and improve the surface finish and for achieving geometric accuracy.

So, if we want to facilitate high-speed machining, a CAM system should be the following:
  • reduce the feed rate loss
  • Achieving a sustainable chip load
  • Increasing the processing speed of program/software
 

ChrisAttebery

Rocket Nerd
Registered
Joined
Jan 11, 2018
Messages
118
Yup, Fusion360 is a very good CAM tool. It can be a little quirky at times.

I'm not in love with the CAD side, but I've been doing integrated circuit layout for over 20 years so I'm kind of set in my ways. ;^)
 

bakrch

H-M Supporter - Gold Member
H-M Supporter - Gold Member ($25)
Joined
Nov 24, 2018
Messages
75
Yep, I use Fusion 360 at home even though I have a mastercam seat (for work).

Lars Christensen has a great YouTube channel showing how to use it, although I think he stopped posting new videos recently. Still, plenty of content there.
 
Last edited:

hman

Active User
H-M Platinum Supporter ($50)
Joined
Feb 17, 2013
Messages
2,374
Thanks for the suggestion! I'm just starting out in Fusion myself, and plan to glom onto these videos.

 

JimDawson

Global Moderator
Staff member
H-M Platinum Supporter ($50)
Joined
Feb 8, 2014
Messages
7,999
Take a look at https://academy.titansofcnc.com/ It's a free online course in CAD, CAM, and machining. The best laid out self paced course I have ever seen, takes you from zero to machining parts in a very short time. Uses Fusion 360, I'm working my way through it to learn the CAD end. Very easy to follow, and understand.
 

Bill MFG

Newbie
Registered
Joined
Aug 16, 2019
Messages
3
I also posted this on cnczone but I'll repost here for those that don't participate there.



I have a G0704 with a 1100W motor on it. I ran it at 4500 rpm for a few years and then bumped it up to 6750 rpm last year. I generally shoot for a MRR of 1.3in/min. I use high quality HSS end mills because they are cheap and these machines don't have the rigidity to use carbide efficiently.

My go to parameters are:
3/8" 2 flute YG-1 aluminum end mill
Speed: 6000 rpm
DOC: .500"
WOC: .05"
Feed: 54 IPM

My general rules for HSM in aluminum are to use full depth, 10-20% WOC, 1-2% feed per tooth. If I need to reduce DOC I increase WOC up to 20%, then I start adding feed. I wish someone made a 3/8" 3 flute in HSS. That would be my next step.

All of this assumes that you have a coolant system of some sort. I use a home brew mist system.

I have used 3/8" 3F carbide end mills in the past. They worked great but cost about 3X what the 3/8" 2F HSS end mills do. I decided that for my needs it wasn't worth the extra expense.

Good luck,


Chris
I appriciate your stance on the cost of carbide, but......
At 3x the cost I'm getting 9x the life. Typically my carbide failes because I failed my carbide. I get aggressive some times. Poor application of coolant causing thermal shock. But I have to say, that 3rd flute is a game changer and as long as your not bone heading it like I do sometimes, they'll last for a VERY long time in aluminum. For me, I like to operate at 80% of adjusted hp. So for a 2hp spindle motor, you'll have 1.8hp at the tool with a belt drive, +/-. So for me, I like to see 1.4ish hp utilization from a 2hp motor. I don't get spindle bog and finish stay nice. It leaves you with enough room to speed up through chatter sometimes, if needed. Gives some maneuvering room with s&f recipe. BTW, I'm running a light machine too. It a Tormach 1100M with ATC and 4th axis. With this small envelope, I use the 4th axis as a horizontal tombstone for more parts per sqr in. I'll try to remember to pull up some of my setting and share them here later. I might be presumptuous in understanding the rigidity of those grizzlies as PM machines, I've not used one. For your smaller tooling(under 3/8") make sure runout is well under .001" . That cost me a few endmill before my head fell out of my 3rd point of contact. Assuming tool holders for these machines are like Mari's.....big mistake.
 

ChrisAttebery

Rocket Nerd
Registered
Joined
Jan 11, 2018
Messages
118
Hi Bill,

Thanks for your feedback. I should have made clear that I was talking about the G0704. It weighs ~300 lbs soaking wet. Your 1100m weighs 1600 lbs according to the spec sheet. I’d love to have one.

The other thing is I’m using a Chinese DC motor that is rated for 1100W(~1.5hp). In reality it’s probably closer to 1hp.

I can watch the column on my mill flex when I’m pushing it with a 3/8 HSS end mill. Adding another flute and carbide isn’t going to help my machine work any harder. I do use carbide on anything under 1/4” though.
 
Last edited:

ChrisAttebery

Rocket Nerd
Registered
Joined
Jan 11, 2018
Messages
118
I had a couple projects in the last week that I really wanted to use a 3/8" 3F end mill on . I picked up a couple Best Carbide 601-33750-1 end mills this morning to try again. They recommend 1200-2400 SFM at .0036 to .0042 IPT. Well, we're going to have to settle for 662 SFM (6750 rpm).

I have a project where I'm cutting two 5.75"x5.75" parts out of a 12x6x.375". They have a large notch out of one corner so I'd like to use adaptive clearing to remove that section. I'm planning to use .375" DOC, .075" WOC, 81 IPM at 6750 rpm. I'll have t do some test cuts and see how these end mills work on my machine. I used a couple of these when I first got my machine running, but I crashed them and decided to stick with HSS. We'll see how they do with the current configuration.
 

bakrch

H-M Supporter - Gold Member
H-M Supporter - Gold Member ($25)
Joined
Nov 24, 2018
Messages
75
I was watching my mill closely the other day and noticed it didn't seem to chatter when conventional milling. I re-posted the toolpaths and the result was a much better MRR and no chatter at all. I kept getting more and more aggressive until my fogbuster nozzle(on a mighty-mag) vibrated so much it wouldn't stay put. The adjustment screw would open itself up as well. The cuts were nice, but vibrations were high, obviously.

Now I have to rip my mill apart when I get a chance, something has to be loose if climb milling is the underdog.

Edit: this test was done @2500 RPM ... .31DOC Axial, .07 Radial .. 64IPM. 4fl 3/8 solid carbide end mill stubby.
 

ChrisAttebery

Rocket Nerd
Registered
Joined
Jan 11, 2018
Messages
118
I did a test starting with the following parameters this morning:
Best Carbide 3F 3/8" Carbide end mill
6750 rpm
DOC .75"
WOC .032"
81 IPM
2"/min MRR

I let the machine run for about a minute and then slowly increased the feed to 98IPM (2.4"/min MRR). The machine was definitely pushing hard. Once I reached 98 IPM the spindle motor popped the 15A/220V breaker it was plugged in to. I reset the machine and continued to cut at 81IPM without a problem. I did follow on tests with the DOC/WOC at .5"/.05", .375"/.065" and .1875"/.130" maintaining the 2"/min MRR. The machine seemed happy enough through all of these test runs.

IMHO at 2"/min MRR my machine is giving me all it is worth. I've had my machine for 7 years. I mostly do prototype/small run parts so saving a few seconds here and there isn't worth as much to me as having reliability and consistency. Occasionally I have a job where I need to hog a significant amount of material away and I'll save these 3 flute end mills for those jobs.
 
[5] [7]
Top