Speeds, Feeds, and Strategies for Bench Top Mills - Page 3


Page 3 of 4 FirstFirst 1234 LastLast
Results 41 to 60 of 65

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

  1. #41
    Member
    Join Date
    Jun 2018
    Location
    on my feet
    Posts
    304
    Downloads
    1
    Uploads
    0

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

    Mitsubishi makes some decent stuff . I love round inserts for their finish and the fact that they can be rotated a lot of times before they are toast .
    You may not have a gear hob but thats going to beat the crap out of putting an indexer on a manual horizontal and cutting a tooth at a time . Your definitely getting some solid machining out of that mill .

    I'll be getting mine back into shape over the next while and plop it between my 440's . A recently purchased 1200w brushless dc should put the stock spindle motor to shame . The motor puts out 5600rpm and I only cut aluminum for the most part so I'll be gearing it for more rpm vs torque , as long as it will pull a 2" facemill at the higher rpm then I'll be happy . The 440's come with the mx3660 , so I'm going to follow the same lines and have a seamless transition to pathpilot



  2. #42
    Member
    Join Date
    Oct 2009
    Location
    USA
    Posts
    376
    Downloads
    0
    Uploads
    0

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

    Quote Originally Posted by CL_MotoTech View Post

    That said, I made another one of these GT750 Water Buffalo (it's a Suzuki) gears, it's for the water pump drive.....Run time is a little over two hours...


    Wow, this is really cool. Do you have any in-progress or workholding pictures?

    So how large is this gear and how wide are the gear teeth? It is hard to tell what scale I'm looking at.

    I tried to CAM up a replacement for a plastic gear in a paper shredder earlier this year, but ran into trouble with the small diameter needed for an endmill to reach the inside of each gear tooth. The problem I had was that endmills small enough to do the gear tooth profile did not have enough cutting length to reach the full depth of the gear teeth. What size endmill did you use to go the gear tooth profile?

    We ended up 3D printing the paper shredder gear, but longevity has been a problem so far. Probably not surprising given that the original paper shredder gear was made of 40% glass fiber reinforced Nylon. Which is why the proper replacement would be aluminum or steel.



  3. #43

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

    Quote Originally Posted by metalmayhem View Post
    Mitsubishi makes some decent stuff . I love round inserts for their finish and the fact that they can be rotated a lot of times before they are toast .
    You may not have a gear hob but thats going to beat the crap out of putting an indexer on a manual horizontal and cutting a tooth at a time . Your definitely getting some solid machining out of that mill .

    I'll be getting mine back into shape over the next while and plop it between my 440's . A recently purchased 1200w brushless dc should put the stock spindle motor to shame . The motor puts out 5600rpm and I only cut aluminum for the most part so I'll be gearing it for more rpm vs torque , as long as it will pull a 2" facemill at the higher rpm then I'll be happy . The 440's come with the mx3660 , so I'm going to follow the same lines and have a seamless transition to pathpilot
    Good luck in your G0704 rehab. I assume that 1200w is continuous and it likely has a much higher peak wattage. If so, you should be pretty good. I run my BLDC at 1:1, it's good for 6k. I ran over drive for up to 8k spindle speed, but with the belleville stack and PDB arrangement I can't get it balanced well enough for that high RPM stuff. So I went back down to 1:1. But without the PDB 8k was great.



  4. #44

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

    Quote Originally Posted by Titaniumboy View Post
    Wow, this is really cool. Do you have any in-progress or workholding pictures?

    So how large is this gear and how wide are the gear teeth? It is hard to tell what scale I'm looking at.

    I tried to CAM up a replacement for a plastic gear in a paper shredder earlier this year, but ran into trouble with the small diameter needed for an endmill to reach the inside of each gear tooth. The problem I had was that endmills small enough to do the gear tooth profile did not have enough cutting length to reach the full depth of the gear teeth. What size endmill did you use to go the gear tooth profile?

    We ended up 3D printing the paper shredder gear, but longevity has been a problem so far. Probably not surprising given that the original paper shredder gear was made of 40% glass fiber reinforced Nylon. Which is why the proper replacement would be aluminum or steel.
    The gear is 3.275" in diameter. The teeth care cut with a 1/16" 3 flute carbide end mill that has .5" of reach. The gear is a .32" thick at the teeth. I start with 4" by 4" by 1" stock, straight in my 4" vise. Once side A is done (the one in the pic above) it gets flipped and held in a three jaw chuck on my table. I probe the ID, then run the other ops.

    I don't imagine milling with anything much smaller than 1/16" would be much fun, not at 6k RPM anyways. It's a slow process, .04" step down, .01" step over. Occasionally i stop the coolant to see if the end mill is still even there. The first few times I machined one I would go in to check and the end mill was gone. Probably washed away into the chip tray.



  5. #45
    Member
    Join Date
    Jun 2018
    Location
    on my feet
    Posts
    304
    Downloads
    1
    Uploads
    0

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

    Quote Originally Posted by CL_MotoTech View Post
    Good luck in your G0704 rehab. I assume that 1200w is continuous and it likely has a much higher peak wattage. If so, you should be pretty good. I run my BLDC at 1:1, it's good for 6k. I ran over drive for up to 8k spindle speed, but with the belleville stack and PDB arrangement I can't get it balanced well enough for that high RPM stuff. So I went back down to 1:1. But without the PDB 8k was great.
    I figure that the 440's set in high have no problem running a facemill at 6000rpm . I can run at 10000 but 6 seems reasonable enough and sounds good . The new motor for the 704 is basically the same set up but larger motor and vfd , so I think a max 8000rpm will be easy to achieve and it would be nice if I can push 10000 . The work I do is mostly finer work so a hogging machine isn't really a necessity



  6. #46

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

    I think 8k or 10k is great if you can do it. Like I said, 8k was great back before I had the PDB. It made running contouring operations an absolute breeze, the machine just whizzed around. If you aren't loading up the spindle hard, you can go for AC bearings too, which should run nice and cool and they generate less parasitic drag. Though I've never had much luck making them last very long. Probably oiling them like I am doing now with the tapered bearings would make a big difference.

    Here's some video. If you watch closely I get some decent sparks coming off the steel at around 37 second to 42 seconds. I upped the f/s by 20%. Finish is still really nice. The Z axis limit switch pooped out though. I'm going to have to rethink my $3 Chinese proximity sensors, at least on the Z. It seems it fails about every 6 months. Perhaps it's vibration related? Either way I am tired of replacing it. Since my ATC is referenced from the limit/homing switch on Z, every time i change the switch I have to adjust the tool change macro.





  7. #47
    Member
    Join Date
    Jun 2018
    Location
    on my feet
    Posts
    304
    Downloads
    1
    Uploads
    0

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

    that sounds great , the spindle loads up some as expected on engagement but overall perfect .

    I swapped out my bearings pretty much from the get go and they've held up well . The spindle has a lot less resistance than the original setup



  8. #48

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

    If you hear that background noise, that's actually the tools rattling in the ATC carousel. This is a result of that balancing issue I still fight with the PDB. Under 5k, everything is great. If I push to 6k, I get a nice resonance. It doesn't seem to hurt cut quality, but I sure would like to minimize it. To be fair, the ATC amplifies it, it's hanging out there 20" from the spindle. I guess I get to use that amplification as a tool for working on this issue.

    I returned to tapered bearings from years of AC's. I think the tapered bearings ultimately are better, once I started loading the spindle hard the AC's just did not last, even very expensive bearings with awesome grease simply couldn't take it. I was changing them every 6 weeks or so. To get the tapered bearings working took some playing. My total loss oil system for the spindle bearings is very simple, but also pretty unique for a G0704 as far as I can tell. I am working on two years on the current set of no-name $20 tapered bearings, every once in a while I get the urge to adjust them, but they never need it once I start tinkering. Two sets of NTN tapered bearings sit in a drawer waiting to make my spindle better yet.



  9. #49
    Member
    Join Date
    Jun 2018
    Location
    on my feet
    Posts
    304
    Downloads
    1
    Uploads
    0

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

    a bit of extra noise is to be expected . The sheet metal covers on all my mills add an amount of excess noise because of vibration . Especially my torus , but it's also bigger with bigger covers . Lots of insulation in my chilling room helps block most of that noise while I sit and watch movies



  10. #50
    Member
    Join Date
    Oct 2009
    Location
    USA
    Posts
    376
    Downloads
    0
    Uploads
    0

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

    Quote Originally Posted by CL_MotoTech View Post
    The gear is 3.275" in diameter. The teeth care cut with a 1/16" 3 flute carbide end mill that has .5" of reach. The gear is a .32" thick at the teeth. I start with 4" by 4" by 1" stock, straight in my 4" vise. Once side A is done (the one in the pic above) it gets flipped and held in a three jaw chuck on my table. I probe the ID, then run the other ops.

    I don't imagine milling with anything much smaller than 1/16" would be much fun, not at 6k RPM anyways. It's a slow process, .04" step down, .01" step over. Occasionally i stop the coolant to see if the end mill is still even there. The first few times I machined one I would go in to check and the end mill was gone. Probably washed away into the chip tray.

    Thanks for that gear info. Now I’m going to take another swing at my paper shredder gear.

    I think I need some 1/16” carbide endmills that have such a long cutting edge. Lakeshore Carbide has a long length 4 flute 1/16” coated endmill for about $16. Is there a better place to get endmills that I’m going to destroy?

    If you think 6000 RPM is slow, then you would be hating life with my Novakon Torus 4500 RPM spindle speed.



  11. #51

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

    I am fairly certain this is the end mill I am using. I do the second round of roughing with a 1/8" end mill as to reduce the amount of time I need to run the 1/16" mill. I also considered drilling the root of each tooth and then milling into that, but I think that method is more trouble than it's worth.

    https://www.ebay.com/itm/1-16-0625-C...351e%7Ciid%3A1



  12. #52
    Member
    Join Date
    Jun 2018
    Location
    on my feet
    Posts
    304
    Downloads
    1
    Uploads
    0

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

    Kyocera are good quality cutters , I've never used them on steel , but , I've got a good stock of their cutters for my work and they do well .



  13. #53
    Member
    Join Date
    Oct 2009
    Location
    USA
    Posts
    376
    Downloads
    0
    Uploads
    0

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

    Quote Originally Posted by CL_MotoTech View Post
    I am fairly certain this is the end mill I am using. I do the second round of roughing with a 1/8" end mill as to reduce the amount of time I need to run the 1/16" mill. I also considered drilling the root of each tooth and then milling into that, but I think that method is more trouble than it's worth.

    https://www.ebay.com/itm/1-16-0625-C...351e%7Ciid%3A1


    Another question for that gear. When you did the backside and indicated the hole for position, how did you get the gear to be rotated at the right angle?

    Thanks for that link. I just bought the last one according to them. Also picked up a Kyocera 3F 1/16” with 3/8” LOC and a 1/4” shank that may be a little more durable for my initial bumbling. Kyocera 1700-0625.375A1. Only an extra $10.50 since all additional cutters ship free.

    https://www.ebay.com/itm/1-16-0625-3...&ul_noapp=true


    So this is the next stage? Starting to pay big bucks to begin stocking up on cutters? It just never ends...

    Last edited by Titaniumboy; 09-26-2020 at 02:17 PM.


  14. #54

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

    When I do the backside I generally forgo the chamfers on the radial holes. That means I don’t have to worry about orientation. That said, I have done it before. To do that, I probe the center and set WC0 there. Then I turn off “set WC0” (not exact verbiage but that’s the effect) in ProbeIt. Then I probe a radial hole, usually Y+ (depends on your CAM setup), if it is off on X then I turn it slightly. I repeat until I get it close, usually like +/-.003 is good enough for me. It takes a couple of cycles because keeping the gear semi loose in the 3 jaw means WC0 will move some when rotating the gear. I hope that makes sense.

    Also, yes buying tools is something that seemingly never ends. When the world ends let’s hope we can trade carbide for food.



  15. #55
    Member
    Join Date
    Oct 2009
    Location
    USA
    Posts
    376
    Downloads
    0
    Uploads
    0

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

    Quote Originally Posted by CL_MotoTech View Post
    When I do the backside I generally forgo the chamfers on the radial holes. That means I don’t have to worry about orientation. That said, I have done it before. To do that, I probe the center and set WC0 there. Then I turn off “set WC0” (not exact verbiage but that’s the effect) in ProbeIt. Then I probe a radial hole, usually Y+ (depends on your CAM setup), if it is off on X then I turn it slightly. I repeat until I get it close, usually like +/-.003 is good enough for me. It takes a couple of cycles because keeping the gear semi loose in the 3 jaw means WC0 will move some when rotating the gear. I hope that makes sense.

    Also, yes buying tools is something that seemingly never ends. When the world ends let’s hope we can trade carbide for food.

    Oh, that makes sense. For some reason I was thinking you had to finish milling the gear teeth from the backside, but your 1/2” long cutter definitely reaches the whole tooth depth from the front side. Just no chamfers on those gear teeth, ha ha.

    Maybe we can trade machine time for food. Those lower receivers aren’t going to make themselves.



  16. #56

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

    Yeah, the teeth are fully machined at that point. I generally chamfer the teeth by hand with a file. I should be able to do the chamfer in process but I’ve never figured the CAM out.

    My coworkers are always asking me to machine lowers for them. I’ve never machined one. It seems like finishing a cast one would be simple. I’ve seen some pretty wild billet ones. That might be fun.



  17. #57
    Member
    Join Date
    Oct 2009
    Location
    USA
    Posts
    376
    Downloads
    0
    Uploads
    0

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

    Quote Originally Posted by CL_MotoTech View Post
    Yeah, the teeth are fully machined at that point. I generally chamfer the teeth by hand with a file. I should be able to do the chamfer in process but I’ve never figured the CAM out.

    That is strange. I would think the chamfer would be the easiest part to CAM. Sayeth the guy who has one part to his name.


    My coworkers are always asking me to machine lowers for them. I’ve never machined one. It seems like finishing a cast one would be simple. I’ve seen some pretty wild billet ones. That might be fun.

    California, bless their hearts, took all the fun out of machining lowers. You have to apply for a California issued serial number before you even start on the 80% conversion. And that is just the beginning of the hoops to jump through that no other state, except for maybe Maryland and NY, requires.

    As you already know, machining lowers for others is a no-no. You just get to machine lowers for your own personal use. Damn shame, it would be fun to machine a whole scad of lowers for friends and family.



  18. #58
    Member
    Join Date
    Jun 2018
    Location
    on my feet
    Posts
    304
    Downloads
    1
    Uploads
    0

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

    easiest thing I've found for chamfering is to run a profile with a tool diameter of .02 and set the depth according to how much chamfer is needed . I use spot drills , so having a pointed tip .01"away from the edge is plenty distance



  19. #59

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

    For the chamfer I really just want the OD of each tooth chamfered. Since that outside diameter isn't continuous on account of the teeth, Fusion didn't really like picking it up. So I gave up. I could probably try harder.



  20. #60
    Member
    Join Date
    Jan 2012
    Location
    USA
    Posts
    52
    Downloads
    0
    Uploads
    0

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

    Popped in here while trying to figure out what I am going to do with my G0704 that has been sitting for years (I got a much bigger industrial machine not long after I converted it) but 5-10% of diameter stepover, 1xD with 3/8" or smaller tools. If you can afford it, get a copy of HSMAdvisor hobby (it's limited to 3HP). You would be surprised at what you discover looking at MRR, cutting forces and HP/torque requirements for a given stepover and DOC.

    A 1/4" carbide 4 flute, at .02 stepover and .25 DOC running at 10k RPM and ~250 IPM in 1018 steel is only using about 1HP with a cutting force of less than 50lbs.

    Your .55" deep cut in aluminum with a 3/8 end mill, 6k RPM, .15" stepover and 55IPM actually requires slightly more HP and a slightly higher cutting force. The cutting forces and HP are similar = you can go faster in steel than you are.

    Make sure you are running tools with the least amount of stickout possible. The TTS holders add a significant amount of stickout and thus leverage on the head and spindle vs R8 collets.



Page 3 of 4 FirstFirst 1234 LastLast

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
  •  


About CNCzone.com

    We are the largest and most active discussion forum for manufacturing industry. The site is 100% free to join and use, so join today!

Follow us on


Our Brands

Speeds, Feeds, and Strategies for Bench Top Mills

Speeds, Feeds, and Strategies for Bench Top Mills

Speeds, Feeds, and Strategies for Bench Top Mills