559,945 active members*
2,015 visitors online*
Register for free
Login
IndustryArena Forum > MetalWorking > General MetalWork Discussion > Acer Vertical Mill w/ CNC retrofit Proper Feeds and Speeds for Plastic Cutting
Results 1 to 3 of 3
  1. #1
    Member
    Join Date
    Jan 2022
    Posts
    2

    Acer Vertical Mill w/ CNC retrofit Proper Feeds and Speeds for Plastic Cutting

    Hi, I'm very new to CNC milling (have some experience with CNC waterjet cutting) and am having some trouble with the proper feeds and speeds for cutting plastic. My machine specs are below:

    Model: Acer E-Mill 3VS II Vertical Turret Mill
    CNC Retrofit: 3-Axis Acu-Rite MILLPWR G2 CNC Retrofit Kit

    I'm trying to cut 4 through holes (0.64" diameter) in a hollow plastic polycarbonate box, around .125" thick. I started out with the below setup:

    Tool: 3/8" diameter downcut end mill
    Plunge Feed Rate: 10 IPM
    Cutting Feed Rate: 10 IPM
    Spindle RPM: 1200 (max my machine can do is 4500)
    Cutting Direction: CCW
    Step depth per Pass: 0.0625

    This setup is pretty slow and probably highly inefficient, and makes a screeching sounds when cutting, so I was wondering if anyone would be able to recommend some better feeds and speeds? I know it would probably make more sense to use a 5/8" diameter bit instead of a 3/8" so if anyone could recommend some feeds and speeds for that diameter end mill as well that would be great.

  2. #2
    Community Moderator Jim Dawson's Avatar
    Join Date
    Dec 2013
    Posts
    5614

    Re: Acer Vertical Mill w/ CNC retrofit Proper Feeds and Speeds for Plastic Cutting

    With an end mill I would use a spiral ramp (about 1degree ramp) and cut the full 0.125'' depth in one step down if the hole diameter is critical. But I really think the proper tool for this job is a step drill. I have a similar machine, and have a similar job coming to do tomorrow where the holes are 0.875''. I'm going to use a step drill.

    I'm not sure a down cut end mill is the correct tool for this job. I think a really sharp standard bit would be a better choice. 3/8'' bit is fine, as is the RPM,I tend to cut plastics at a bit slower SFM than most people to keep it from melting. But I might bump the feed speed to 20 IPM to increase the chip load. Like mine, your machine, or any knee mill, is not well suited for high feed speeds. If I were doing this in my Haas, I would be using about 150 IPM feed and bump up the spindle speed to maintain about a 0.004'' chip load. I would not use a 5/8 end mill, maybe a 1/4'', 2 flute.

    If you can properly support the working surface on a spoil board it will help with the chatter.
    Jim Dawson
    Sandy, Oregon, USA

  3. #3
    Community Moderator Jim Dawson's Avatar
    Join Date
    Dec 2013
    Posts
    5614

    Re: Acer Vertical Mill w/ CNC retrofit Proper Feeds and Speeds for Plastic Cutting

    Quote Originally Posted by sarahn27 View Post
    That's very helpful, thanks so much Jim! By standard bit, do you just mean a regular drill bit?

    And for the step bit, is there a specific one you recommend? If I used the step bit, could I just plunge the full depth until I reach the 0.625 diameter step? Or would I do the drilling in stages (plunge to the .25 diameter, retract then the .5, retract then the final .625 for example)?

    Also what would be the highest RPM you would try for plastic? I have 200 of these boxes to mill (800 holes total) so I'm just trying to be as efficient as possible.

    But yeah the work holding is definitely not the best set up. I'm milling into the side of the hollow box so the face I'm drilling into is not supported on the other side. Do you think this is the main cause of the screeching? I was debating putting a block of wood inside the box to support the wall I'm drilling into but not sure if that'd be worth it.

    No, not a drill bit, but a standard endmill, up cut. Highest RPM? I would start a bit slow and bump up both the feed and speed until it becomes a little squirrelly then back it down a bit. Every job is different.

    No specific recommendation on step drill brands, but spend about $30 on a good one, the cheap ones are junk. If you are in the USA, Home Depot sells Kline tools in the electrical department.

    I think just plunging in with a step bit is what I would do. No peck drilling needed. If you can get away with a 0.625 hole, then this becomes really easy with a step drill. If you need a 0.640 hole then milling is most likely the best way to do it. An option would be a 41/64 (0.64) drill bit, ground for plastic so it doesn't try to catch and rip the box apart. It's easy to modify a standard drill bit for plastic use. Google ''drilling plastic'', there are a lot of good tips out there.

    Yes, I think you need to support working surface of the box, wood is fine for this application. I would build a proper fixture to hold and locate the box, and secure it with a toggle clamp. For drilling, it doesn't require much to hold it in position. Milling requires better clamping. I'm sure the chatter you are hearing is due to the unsupported box.
    Jim Dawson
    Sandy, Oregon, USA

  4. #4
    Member
    Join Date
    Jan 2022
    Posts
    2

    Re: Acer Vertical Mill w/ CNC retrofit Proper Feeds and Speeds for Plastic Cutting

    Hi Jim,

    Your recommendation worked well, so thank you! I have to cut three more materials (listed below), would you be able to give me some starting recommendations for them? Thank you!

    1) High Strength 2024 Aluminum
    2) Multipurpose 6061 Aluminum
    3) Low-Carbon Steel

  5. #5
    Community Moderator Jim Dawson's Avatar
    Join Date
    Dec 2013
    Posts
    5614

    Re: Acer Vertical Mill w/ CNC retrofit Proper Feeds and Speeds for Plastic Cutting

    First you need to take into account the limitations of your machine. As I said above, a vertical turret mill is not a production machine and you can't expect it to do the work of a production machine. You have a 3V frame machine, and mine is a 4V frame, about 1000 lbs heavier than yours. Same HP and head. I normally use 1/4'' to 1/2'' cutters on mine depending on the job. 1/2'' cutters are about all the machine will take and still remain stable. There are times I have used larger cutters when a lot of stick out is required, but the feed speed and depth of cut needs to be adjusted for the larger diameter cutters.

    For all practical purposes the 2024 and 6061 can be treated the same. I prefer aluminum cutting 2 or 3 flute carbide endmills, about 40% step over, up to 2X dia for depth of cut, and a chip load of 0.001'' to 0.002''. Adjust the feed speed to what the machine will take and the RPM to meet the chip load requirement. There is no way you can exceed the SFM limitation of the endmill. Spray mist coolant. I have never worked with 2024, but I understand that it is less gummy than 6061 and thus a bit nicer to work with.

    For mild steel, you can pretty much treat it like aluminum. I normally use 4 flute carbide endmills designed for steel cutting. Again adjusting the feed and speed to maintain a 0.001'' to 0.002'' chip load. Maybe 30% step over and a bit less depth of cut. Spray mist coolant.

    In either case, you can feel when the machine is happy. I normally use feed speeds in the range of 5 to 30 IPM. If it starts vibrating you are pushing it too hard, if you are getting a lot of chatter, then try a bit more feed speed or a bit lower RPM. You will notice I did not address SFM, you will always be below the limitations of the end mill, the chip load is the important parameter. You need a heavy enough chip load to make sure the tool is cutting and not rubbing, but you also need to stay within the limitations of the machine.

    If we were having this discussion about a production machine, then all of the suggestions above would be different.
    Jim Dawson
    Sandy, Oregon, USA

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
  •