Speeds, Feeds, and Strategies for Bench Top Mills

I finished this shift lever up. Still working on those feeds and speeds for the steep and shallow, but the back side turned out really nice.

I roughed at .5" DOC, .003" fpt, at 54 ipm with a carbide 3 flute end mill. Still not chatter, all is well. The end mill is pretty tuckered out too. It has about 1 decent cutting edge left, one was knocked off on a clamp (separate project), the other was chipped off when I dropped the end mill and tool holder. All the finishing was done with a 2 flute 3/8 cabride ball end. I ran that at 36 ipm.

My Bellevile arrangement ended up using two different stiffness washers to form a progressive stack. That allows me to tighten the drawbar to where the majority of the washers are basically flat when the tool is release, but the stiff set allow a bit of over travel, hopefully preventing damage to the actuator, mounts, drawbar lever. My stack is also fairly large, I'm using 24 of one time and six of the other.

https://i.imgur.com/ZmBBCSz.jpg

https://i.imgur.com/wh6LQfF.jpg

Looks nice that :)

All I've got done on my AMAT25LV (PM25) is a couple of slot tests.
So far tried a 3flute 8mm end mill chinese £1 jobbie lol.
2500rpm, 450mm/min, 3mm doc, cut like butter and no rpm fluctuations or chatter! used no coolant either.
Will up it at next test.

My Sieg X2 would have stalled straight off at 1.2mm doc even with flood!!!!
WHY did I waste my time with that pos!!!!! Wish I'd just gone straight in with one of these bigger mills!!

Are you still with R8 or have you moved to TTS? I took an immediate step backwards when I moved to TTS, which prompted this thread for me, but as I've gotten my PDB and belleville arrangement worked out I've clawed my way back to R8 performance territory. The mill itself is definitely the weak point now. You can definitely push it harder than 3mm DOC, but slotting is taxing. 10mm DOC with a .08mm (converting from imperial to proper units just by feel so don't take these numbers too seriously) chip load should be doable without too much trouble. Keep in mind full engagement will require much slower feeds and less chip load.

I try to avoid slotting, generally I will go down a tool size and then rework my CAM to get a toroidal tool path. It ends up being somewhat slower but tool life is better. I'm not really in a rush with this machine, fast just doesn't really happen. Though the 2.2kw spindle and ATC have changed the game. I no longer worry about stalling the motor and can walk away during multi-tool machining. That said, I am still learning. Every time I run the machine I learn something new. I have gotten to the point where I can make many things without breaking stuff, but still the machine can make me feel like it is "amateur hour" if I'm not careful. It's a humbling experience to be honest.

As for coolant, when my coolant pump died I was running quite a number of parts without it. I was very surprised how nice the finish was with the 6061 I was working with. I think coolant isn't as necessary as long as you can generate the chip load to cool the tool and the stock. The finishing pass might be tough as the chips are too thin to pull the heat out of the tool? I'm not sure. I switched to flood coolant early in my CNC conversion and never looked back. Maybe erroneously so.

I haven't updated in a while but I am still plugging along. Most recently I had some steel projects, which are very rare for me. So I pretty much was starting from zero with speeds and feeds. Nevertheless, the Harvey F&S chart was utilized and I bought a couple of .25" 4 flute Tin coated carbide end mills (Kyocera) from McMaster. Well, the machine chugged right along and so far I have had great luck. Since I don't have a clue what type of DOC I can manage I started pretty conservative, but I'm now up to .15" DOC and am running .035" WOC. I've done this on some hardened steel gears as well as some cheap steel plate I bought off eBay. Results have been great and end mill life is very good. On the gears I managed +/-.00025". Way better than I expected, but I did run finishing passes with very patient (slow, perhaps painful, 8ipm) speeds. I have 10 or more hours on one end mill and it looks new. I'm sure I can run a bit harder yet. One of the funnest experiments was to run my 2" shell mill and square the stock. Bright red molten steel was flying off in all directions, this was a new experience for me and I really enjoyed it. I wish I had gotten a picture. Surface finish was very nice, perhaps only limited by the flexibility of my G0704, but still very fine on the finger nail. There were no noticeable ridges. I have a lot to work on with my technique and understanding of machining steel, but so far so good. The little mill, homemade drawbar, TTS, ATC, it's all starting to exceed my expectations.

kyocera makes some nice tools . Check out gorilla mill , they cost a bit more than the typical brands but the savings is in the longevity of their working capabilities . They make the best cutters I've ever seen for milling any steel . I turned a buddy in a gear shop onto those and they never turned back . They also have good speed and feed calculations for their mills

Cool! I'll check that brand out!

I have been using these carbide 3 flute 3/8" end mills in aluminum that I get from ebay. When they are new my god do they ever cut, but they are insanely brittle, and they seem to dull after just a few hours of run time. 6 hard hours and they are chopping away. When they are brand new, the cut hardly makes a noise.

I guess what I am learning is that end mill brand matters.

brand and grind are important . A general endmill with a coating isn't going to keep up to a quality variable flute/helix . These variables prevent the tool from forming harmonics and chatter . There are a lot of brands that fit the bill , but , I have never come across another brand that has a harder carbide than gorilla , and it's evident while grinding a setscrew notch

I have a PM25, but I built a new headstock and put a 12K RPM 3.0KW spindle on it. So my numbers aren't directly comparable vs a stock machine.

However the stiffness problem is still the same. What has worked best for me on most metals, is high RPM, high DOC, about 10% stepover, and a moderate chip load. For steel, I can remove about .5 cubic inches/minute with a 1/8 end mill doing this. In aluminum, I've gone up to 3 cubic inches/min, but that is not a comfortable speed.

To anyone with a stock spindle, I recommend max RPM, DOC = diameter or more, 10% stepover, and start off with a light chipload and work your way up till you find what works best. Keeping the DOC high seems to work better than any other thing I've tried, seems to reduce vibration keeping the cutter engaged all the time into the material.

My go to is 1/4" end mills, but I've run 3/8 and 1/2" ones too. 1/4" is just easy, makes CAM easy for a lot of the work I do.

You can probably do better than that in Aluminum, especially with the available RPM have (assuming you have the torque). I used to run my spindle over-drive for 8k, but the vibration was too much when I added the power draw bar. I'm still refining the PDB so I may revisit 8k someday.

I rough at 6000 RPM (spindle max), .55" DOC, .15 WOC, .003IPT, with a 3/8" 3 flute Zrn carbide end mill. That gives 4.5 cu. in per minute and I feel very comfortable running that.. I've run harder, running as much as .65" DOC for 5.3 cu. in. per minute, but the mill is definitely getting a bit noodly at that point. You have get your ways (assuming you still have ways) really good and tight to get above 4 cu. in. per minute, IMO. In the Chris Attebary G0704 thread we talk about these F/S and he experienced the same results after working on his ways. The cuts are nice and quiet, no drama. Just the way they should be, and for such a small machine with generally small work pieces, you make quick work of stock at these rates.

3/8" end mills have become my go to for most aluminum projects, but 1/4" and 1/8" get used fairly often too. I have one project that is 4 hour run time with a 1/16" end mill. The ATC has helped with this, i used to avoid tool changes like the plague.

Show off that 12k spindle setup, I'd love to see that.

It can probably do more, I just haven't pushed it to be honest. I use this occasionally, often when not making a mistake is more important than cycle time or cutter life. I would like to do some test cuts one day and learn what it'a actually capable of though. My VFD is only a 2.2KW, so that is what limits my power. Would like to upgrade that one day.


Here's a couple pics.

https://i.imgur.com/4tPWnXT.jpg

https://i.imgur.com/SzRW64v.jpg

Nice!

What are those headers for? That must be pretty small 4 cylinder to fit on a PM25. I did the heads for a G750 and it took up more X than that header.

https://i.imgur.com/KDLpqqZ.mp4

https://i.imgur.com/5xSdZtx.jpg

I’ve run into an issue with the X axis that is rather curious. Basically, the X axis won’t move without stalling the stepper. Thinking I probably smoked the driver I decided to switch the X stepper onto the Y driver. Sure enough, it ran smoothly. However, both the Z and Y axis run fine off the X axis driver. So, the driver seems fine, and the wiring and plug seem fine. But if I put the X axis stepper back on the X axis it immediately starts chugging along with basically non stop step loss, and it occasionally switches directions while in movement. This indicates to me that I’m not getting solid contact across the all stepper inputs. So, right now I am thinking this has to be the plug on the X stepper cable. It makes good contact on the YZ outputs, but not on its output. If it were the cable, it would be an issue on all drivers. If it were the driver, all axis would lose steps when plugged in.

If anybody has other ideas let me know, otherwise I am going to replace the plug on the X axis cable and see what happens.

I got to work on this tonight and sure enough one of the contacts on the X axis stepper side plug was looking pretty burnt. I replaced the plug with a new one and it seems like the issues are solved. There’s a good chance these no-name DB9 plugs just aren’t up to the amperage I am running, but I am on year 6 with them so I think I’ll stick it out a bit longer before looking for other options. While I was in there, I took the time to clean up some of the other wiring, just routing issues mostly. Tomorrow I will get everything back together and give it a good run. I have some more steel to machine so it should be good fun.

After repairing the plug and running the machine for a few hours the thing stopped dead in its tracks. The MX3660 burnt up and was showing a persistent error. I purchased a new one and tossed it in. A direct replacement makes for an easy repair. It took maybe 25 minutes. I used the opportunity to clean the chip tray that was way over-full. I also extended a few of the cables that were too short with the new enclosure, this just makes it easier to get the controller connected up. Also, while i was in the enclosure I added another fan. The G540 always got pretty warm, but I never paid much attention to the MX3660. There's a new fan in there to hopefully do something...

After doing those revisions I cleaned the enclosure and checked calibration on the axis. All is good! The calibrations were spot on after changing the drivers. After about two weeks of no machining I am back! I have more steel to do, and several customer orders in aluminum. Temperatures here have fallen into the low 70's during the day, and I really am looking forward to making things in a shop that isn't 100F.

Beyond those customer parts I have a revision to the power drawbar all drawn up. 6 months in on the prototype and I pretty much know where its weak spots are. It's still working well in the prototype form, but I can tighten the entire design up and make it iron clad with some minor revisions.

After I get a few more hours in on the machine I will update some feeds and speeds. I think I am getting close to another jump in performance.

Well, I got a good crack at some steel this evening. And I had a good run on some aluminum yesterday. In Al, all is well. The new MX3660 seems to have actually improved my performance some. My guess is that the Y axis drive was faulty for some time.

For the steel work I ran my 2" 4 flute round insert (10mm) face mill. I ran it at 5000rpm at 20ipm and .001" fpt. The stepdown was .02", and optimal load was .8". This gives around .3 cubic inch per minute volume. Not fast, but the result were very good. There is certainly more left in the machine, but I took it easy. The finish on the flat surface was very nice considering I wasn't trying to make a nice surface, and the operation ran drama free. I've run higher chip load in steel, enough to get the chips red hot with this face mill, but I wasn't in a hurry here and each operation was only around 20 minutes. So there wasn't much to gain. At the end I increased feed to 110% just to see, it certainly wasn't stressing the machine out. I ran full flood, I still have some confidence to gain without flood. But I think I'm sending enough coolant that I should be okay with these slow feeds and speeds.

https://i.imgur.com/vuACJGk.jpg

https://i.imgur.com/aNpeWpU.jpg

looks good and nice finish
the rates and depth of cut were a wise choice with all things considered . With that much stick out the part would likely be singing with more depth of cut . I've always been a fan of taking light depths of cut with high rpm and feed rates

I had considered throwing a larger vise on the table or perhaps a set of 2" soft jaws in that one, but got lazy. It did sing a tad bit when at full load. Not enough to worry about though.

I have another 1000rpm of spindle speed, so next time I will probably take advantage that extra 20% and add some feed next time around.

Overall, I am pretty happy with it. I am not a fan of cleaning up steel chips though. Aluminum does a much better job of collecting in my chip tray.

steel is always a mess to clean up . For the diameter of tool and your chip load I'd think your in a sweet zone , obviously depending on the grade of insert . Faster rpm might cause your cutter to break down sooner . I'd look at upping the feed rate in increments until finding that sweet spot

The face mill is a "Mitsubishi" 2" face mill with 10mm round inserts that are also from "Mitsubishi". I bought it for like $60 on eBay years ago.

I am on the first set of inserts, though I recently turned them about 30 degrees. Knockoff or otherwise, it works really well. It's a horsepower hog, which I have plenty of, but ultimately the G0704 decides when it's had enough and I have to back off.

That said, I made another one of these GT750 Water Buffalo (it's a Suzuki) gears, it's for the water pump drive. The OEM plastic ones like to fall apart. My father and I have a rather wicked GT750 powered vintage race car and I developed this gear for that. It's been an unexpected hit, I sell a few each month right now. They go the world over. Run time is a little over two hours, I'm told the gear could be hobbed in minutes. I don't own the equipment, so here we are.

https://i.imgur.com/UN6xtfd.jpg

https://i.imgur.com/7VvCx2Y.jpg

Looking at those pics, I need to clean these parts better after machining. haha