525,444 active members*
2,670 visitors online*
Register for free
Login
IndustryArena Forum > MetalWorking Machines > Benchtop Machines > Speeds, Feeds, and Strategies for Bench Top Mills
Page 2 of 2 12
Results 21 to 31 of 31
  1. #21

    Re: 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.




  2. #22
    Registered
    Join Date
    Jan 2018
    Posts
    509

    Re: Speeds, Feeds, and Strategies for Bench Top Mills

    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!!

  3. #23

    Re: Speeds, Feeds, and Strategies for Bench Top 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.

  4. #24

    Re: Speeds, Feeds, and Strategies for Bench Top Mills

    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.

  5. #25

    Re: Speeds, Feeds, and Strategies for Bench Top Mills

    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

  6. #26

    Re: Speeds, Feeds, and Strategies for Bench Top 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.

  7. #27

    Re: Speeds, Feeds, and Strategies for Bench Top Mills

    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

  8. #28

    Join Date
    Sep 2018
    Posts
    13

    Re: Speeds, Feeds, and Strategies for Bench Top Mills

    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.

  9. #29

    Re: Speeds, Feeds, and Strategies for Bench Top Mills

    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.

  10. #30

    Join Date
    Sep 2018
    Posts
    13

    Re: Speeds, Feeds, and Strategies for Bench Top Mills

    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.




  11. #31

    Re: Speeds, Feeds, and Strategies for Bench Top Mills

    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


Page 2 of 2 12

Similar Threads

  1. Replies: 3
    Last Post: 12-08-2017, 12:42 AM
  2. HDPE feeds, speeds and mills
    By Erant in forum Glass, Plastic and Stone
    Replies: 0
    Last Post: 10-07-2015, 09:01 PM
  3. Speeds and Feeds/Small End Mills
    By Magnum164 in forum Tormach Personal CNC Mill
    Replies: 16
    Last Post: 02-13-2015, 07:45 AM
  4. End Mills and Feeds n Speeds
    By Simon Wells in forum CNC Tooling
    Replies: 39
    Last Post: 03-20-2012, 06:11 PM
  5. Opinions needed on cnc bench top mills
    By M4RK_23 in forum Benchtop Machines
    Replies: 16
    Last Post: 01-10-2006, 05:48 AM

Tags for this Thread

Posting Permissions

  • You may not post new threads
  • You may not post replies
  • You may not post attachments
  • You may not edit your posts
  •