Slotting with 1/8" cutter, need suggestions on speeds/feeds
Close
Login to Your Account
Page 1 of 2 12 LastLast
Results 1 to 20 of 33
  1. #1
    Join Date
    Apr 2021
    Country
    UNITED STATES
    State/Province
    California
    Posts
    8
    Post Thanks / Like
    Likes (Given)
    5
    Likes (Received)
    0

    Default Slotting with 1/8" cutter, need suggestions on speeds/feeds

    Beginner CNC machinist here. Trying to cut 1/8" slots in 1/8" cold rolled steel. Not going well.

    Using 4 flute carbide EM, 1/4" flute length. 4000 RPM, .042 DOC, .0003 feed/tooth. Based on info from Harvey tool site.

    I can ramp in OK, but attempt today the cutter broke after about a 1/4" into slot.

    Thinking i need to reduce the DOC. Even with the small feed/tooth the cutter may be loading up? I'm using a mist cooler.

    I've had some success with a 3 flute. Maybe it was just luck. Thinking 4 flute should be stronger.

    Please give me your suggestions.

    Thx.

    Marty

  2. #2
    Join Date
    May 2010
    Location
    BainBridge IS
    Posts
    12
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    38

    Default

    Quote Originally Posted by SkeeterWeazel View Post
    Beginner CNC machinist here. Trying to cut 1/8" slots in 1/8" cold rolled steel. Not going well.

    Using 4 flute carbide EM, 1/4" flute length. 4000 RPM, .042 DOC, .0003 feed/tooth. Based on info from Harvey tool site.

    I can ramp in OK, but attempt today the cutter broke after about a 1/4" into slot.

    Thinking i need to reduce the DOC. Even with the small feed/tooth the cutter may be loading up? I'm using a mist cooler.

    I've had some success with a 3 flute. Maybe it was just luck. Thinking 4 flute should be stronger.

    Please give me your suggestions.

    Thx.

    Marty
    If it is a straight slot, can you turn the part 90 degrees and use a carbide slitting saw? Alternatively, use a smaller end mill and an adaptive tool path. This link may be of use. It is slotting with stainless steel with 1/8" end mill: Milling 304 Stainless with a Carbide End Mill | Speeds and Feeds Tool Test - YouTube

  3. #3
    Join Date
    Oct 2010
    Country
    UNITED STATES
    State/Province
    Oregon
    Posts
    5,675
    Post Thanks / Like
    Likes (Given)
    5501
    Likes (Received)
    2153

    Default

    Yeah, when I read the thread title, I immediately thought slitting saw, which should be reasonably robust at 1/8" width. 0.001" per tooth feed for starters. Whatever SFM is appropriate for the cutter and work materials.

  4. #4
    Join Date
    Apr 2021
    Country
    UNITED STATES
    State/Province
    California
    Posts
    8
    Post Thanks / Like
    Likes (Given)
    5
    Likes (Received)
    0

    Default

    Thx for replies. I'm making a router guide plate of sorts, Some slots are curved. After watching video i think i'm not use enough "mist" to flush out chips. I am using a "cheapy" cutter from McMaster Carr. Maybe 3 flute is better. Crap, i hate breaking cutters. If i felt i was learning it wouldn't be so bad. But i feel i'm just shooting in the dark.

  5. #5
    Join Date
    Nov 2014
    Country
    UNITED STATES
    State/Province
    Florida
    Posts
    6,185
    Post Thanks / Like
    Likes (Given)
    2451
    Likes (Received)
    3075

    Default

    Quote Originally Posted by SkeeterWeazel View Post
    Thx for replies. I'm making a router guide plate of sorts, Some slots are curved. After watching video i think i'm not use enough "mist" to flush out chips. I am using a "cheapy" cutter from McMaster Carr. Maybe 3 flute is better. Crap, i hate breaking cutters. If i felt i was learning it wouldn't be so bad. But i feel i'm just shooting in the dark.
    4 flute is stronger, but less room for chips. Maybe a 2 flute for better chip evacuation. I don't like 2 flutes, but without flood coolant... maybe will be better?

  6. #6
    Join Date
    Jun 2011
    Location
    Maine
    Posts
    96
    Post Thanks / Like
    Likes (Given)
    2
    Likes (Received)
    5

    Default

    Osg 5 flute. If you can program it use a trichordial toolpath. I cut .16” wide .10” deep by 1.50” long slots in 316l at 20 ipm 6200 rpm with a .020 stepover. The end mill will run for hours this way. I use the peel mill feature in mastercam. You can also write a simple macro to do this.

  7. Likes SkeeterWeazel liked this post
  8. #7
    Join Date
    Sep 2017
    Country
    UNITED STATES
    State/Province
    Wisconsin
    Posts
    1,285
    Post Thanks / Like
    Likes (Given)
    337
    Likes (Received)
    804

    Default

    If I can I default to high feed milling for situations like this. If not, I'll use a profile ramp with a stepdown limited to around 1/4-1/3 of cutter diameter using a smaller endmill (In this case I'd use a 3mm). I will use a corner radius tool in steel. Chip evacuation is huge - this might sound obvious but make sure you're blowing chips behind the toolpath not in front of it.

  9. #8
    Join Date
    Feb 2007
    Location
    Ontario, Canada
    Posts
    148
    Post Thanks / Like
    Likes (Given)
    295
    Likes (Received)
    19

    Default

    Some other ideas to try after you reduce the DOC: change material to a leaded steel, like 12L14. If this is a project for your own use, spoil yourself and use brass. Also try the first passes with a ball end mill, then clean up with an end mill. And along the way, learn to make "D bit" cutters, essentially a single flute tool (you can make them from the broken Harvey end mills).

  10. #9
    Join Date
    Jun 2011
    Location
    Maine
    Posts
    96
    Post Thanks / Like
    Likes (Given)
    2
    Likes (Received)
    5

    Default

    Check out Harvey’s website they have a section on slotting.

  11. Likes SkeeterWeazel liked this post
  12. #10
    Join Date
    Dec 2015
    Country
    UNITED STATES
    State/Province
    Illinois
    Posts
    591
    Post Thanks / Like
    Likes (Given)
    208
    Likes (Received)
    376

    Default

    Are you using a router, or a HF mill converted to CNC or are you using a real machine tool? It makes a big difference in tool life.

  13. Likes mhajicek liked this post
  14. #11
    Join Date
    Apr 2021
    Country
    UNITED STATES
    State/Province
    California
    Posts
    8
    Post Thanks / Like
    Likes (Given)
    5
    Likes (Received)
    0

    Default

    Guys, thx for your replies.
    Kenton: it is a CNC Masters Supra (?) mill. It’s a Bridgeport clone converted to CNC.
    Rick Finsta: what is high feed milling? Profile ramp? My step down now is 1/3 of cutter diameter.
    Thx.

  15. #12
    Join Date
    Feb 2020
    Country
    UNITED STATES
    State/Province
    Alabama
    Posts
    331
    Post Thanks / Like
    Likes (Given)
    136
    Likes (Received)
    90

    Default

    Quote Originally Posted by SkeeterWeazel View Post
    Beginner CNC machinist here. Trying to cut 1/8" slots in 1/8" cold rolled steel. Not going well.

    Using 4 flute carbide EM, 1/4" flute length. 4000 RPM, .042 DOC, .0003 feed/tooth. Based on info from Harvey tool site.

    I can ramp in OK, but attempt today the cutter broke after about a 1/4" into slot.

    Thinking i need to reduce the DOC. Even with the small feed/tooth the cutter may be loading up? I'm using a mist cooler.

    I've had some success with a 3 flute. Maybe it was just luck. Thinking 4 flute should be stronger.

    Please give me your suggestions.

    Thx.

    Marty
    First of all, there is no such thing as "cold rolled steel". You have hot rolled and cold formed. What type of cold formed steel? There are many varieties with substantial differences. That is why 12L14 was mentioned. It is the best cuttingwise.
    Secondly, your problem is sfpm. Are you at max rpm? Can you double it? What is the Length to diameter ratio of your cutter? If you are more than 2x the ratio you will have to drop your DOC.

  16. #13
    Join Date
    Dec 2015
    Country
    UNITED STATES
    State/Province
    Illinois
    Posts
    591
    Post Thanks / Like
    Likes (Given)
    208
    Likes (Received)
    376

    Default

    Assuming that your cold rolled is in fact 1018 there seems to be something else going on. (I will say cold rolled, it is what I was taught, it is what everyone I know calls it, and I ain't gonna let COVID tell me what to do.)

    If your CNC conversion has any motion control issues they will definitely cause small endmill to die a rapid death. Other issues that spring to mind are checking your tool runout and your tool pulling or slipping in your tool holder. Your speeds, feeds and cut depths are about where I would start on the spindle speed limited Proto-Trak I run at work.

    Edit: if your ramp angle is too steep you could be damaging your cutting edges before you even get a chance to start cutting, causing your rapid tool failure.

  17. Likes SkeeterWeazel liked this post
  18. #14
    Join Date
    Oct 2009
    Location
    Oregon
    Posts
    5,940
    Post Thanks / Like
    Likes (Given)
    6431
    Likes (Received)
    3308

    Default

    Quote Originally Posted by CORONA VIRUS View Post
    First of all, there is no such thing as "cold rolled steel". You have hot rolled and cold formed.
    Huh. Interesting. I wonder if the steel mills that roll steel cold know this?

  19. Likes mhajicek liked this post
  20. #15
    Join Date
    Oct 2009
    Location
    Oregon
    Posts
    5,940
    Post Thanks / Like
    Likes (Given)
    6431
    Likes (Received)
    3308

    Default

    If the tool has square corners that's a problem. Bigger radius the longer it lasts in steel.

    My biggest issue when using 1/8" and smaller endmills is runout. I have bigger machines, rarely run anything under a 1/2" endmill. It's not unusual for me to run an 1/8" EM in a straight shank collet holder in a 50 taper holder. Easy to get a couple thou runout out at the endmill and the tool does about what you experience.

    For a full width slot I don't usually take more DOC than 50% of the diameter to start with. Once the process is proved I'll squeak that up if there's room.

  21. #16
    Join Date
    Sep 2017
    Country
    UNITED STATES
    State/Province
    Wisconsin
    Posts
    1,285
    Post Thanks / Like
    Likes (Given)
    337
    Likes (Received)
    804

    Default

    Quote Originally Posted by SkeeterWeazel View Post
    Guys, thx for your replies.
    Kenton: it is a CNC Masters Supra (?) mill. It’s a Bridgeport clone converted to CNC.
    Rick Finsta: what is high feed milling? Profile ramp? My step down now is 1/3 of cutter diameter.
    Thx.
    High Feed milling uses special tools with a larger radius than the tool diameter allows, and geometry that puts cutting forces axially up into the spindle and down into the workpiece. You take very large chiploads at high SFM and very low depth of cut and very large stepover. They don't remove material like HSM (high speed machining, where you go as deep as possible and take very small stepovers) but it is a very reliable process for slotting, long stickouts, sketchy setups, etc. They are great, but expensive.

    On that type of machine, I would suggest you look at a bullnose 4-5 flute 3mm diameter tool with a reduced shank and very short flute length, and then ramp profile the part with a <1.5-2 degree angle or no more than 1/4 times the tool diameter total depth per pass. By profile ramping with a smaller tool than the slot width you can get away with a little more runout and you also can get better chip evacuation and less recutting.

  22. Likes SkeeterWeazel liked this post
  23. #17
    Join Date
    May 2017
    Country
    UNITED STATES
    State/Province
    Minnesota
    Posts
    1,764
    Post Thanks / Like
    Likes (Given)
    2292
    Likes (Received)
    1171

    Default

    Quote Originally Posted by SkeeterWeazel View Post
    Guys, thx for your replies.
    Kenton: it is a CNC Masters Supra (?) mill. It’s a Bridgeport clone converted to CNC.
    Rick Finsta: what is high feed milling? Profile ramp? My step down now is 1/3 of cutter diameter.
    Thx.
    I'd expect some backlash on that type of machine; you'll have to cut your parameters down significantly from the manufacturer's recommendations.

  24. #18
    Join Date
    Apr 2021
    Country
    UNITED STATES
    State/Province
    California
    Posts
    8
    Post Thanks / Like
    Likes (Given)
    5
    Likes (Received)
    0

    Default

    sample.jpg
    Here is pic of my sample cutting program i did tonight. It encompasses all the features i'll need to do on the real template, aside from the slots will be much longer. The circle on the right i can ramp in OK, as well as the rectangle feature on the left. 1/8" hole at the top i can plunge in. The slot starts from the circle. I changed the program so the slot is taken in 4 passes. Cutter broke half-way through the 4th pass.

    top-burr.jpgtop-burr2.jpg
    Notice the big burr. I think the cutter is loading up. I would think a fresh cutter at these light cuts shouldn't create any burr like this. Looking at the broken cutter there appeared to be some material slightly stuck in the flutes. I could scrape it out, but had to work at it.

    bottom-burr.jpg
    This is bottom side of sample, showing burr.

    Guys, i appreciate your help with this. Please keep suggestions coming.
    Marty

  25. #19
    Join Date
    Aug 2005
    Location
    South Australia
    Posts
    233
    Post Thanks / Like
    Likes (Given)
    26
    Likes (Received)
    46

    Default

    Hi, not a CNCer but if you REALLY do mean 0.0003"/tooth that cutter is trying to RUB its way thro' .. no wonder it broke! Try 0.002" per tooth or 0.003" which I suspect was really the recommendation.

  26. #20
    Join Date
    Apr 2021
    Country
    UNITED STATES
    State/Province
    California
    Posts
    8
    Post Thanks / Like
    Likes (Given)
    5
    Likes (Received)
    0

    Default

    I hear you, but this site is recommending .00039 as a starting point. Remember, this is only an 1/8" cutter.
    link below
    https://harveyperformance.widen.net/...0.pdf?u=r5tz5r


Tags for this Thread

Bookmarks

Posting Permissions

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