CNC Toolpath Strategies for smaller machines

macardoso

H-M Supporter - Silver Member
H-M Supporter - Silver Member
Joined
Mar 26, 2018
Messages
2,724
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.
 
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.

oXiaFZUl.jpg

KqurGKxl.jpg
 
Last edited:
I'd go with a 4 flute end mill and a deeper cut.
 
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
 
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'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.
 
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.
 
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!
 
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.
 
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:
Back
Top