Engraving with a 1/32 ball mill
Largest Manufacturing Technology
Community On The Web
Close
Login to Your Account

Page 1 of 2 12 LastLast
Results 1 to 20 of 21
  1. #1
    Join Date
    May 2012
    Location
    Mid-Iowa, USA
    Posts
    3,510
    Post Thanks / Like
    Likes (Given)
    3401
    Likes (Received)
    2032

    Default Engraving with a 1/32 ball mill

    Exactly as the title states. Material is 304 laser cut, machine is a Haas VF-6SS with a 12k spindle. Obviously spinning at 12k, but what would everyone's feed be at .01" deep? HSMAdvisor always seems to me to be very low on these numbers (1.41 IPM? Yes this is with chip thinning turned on). Tool has a 1/4" shank and a real short flute length, solid carbide AlTiN coated.

  2. #2
    Join Date
    Dec 2014
    Country
    CANADA
    State/Province
    British Columbia
    Posts
    621
    Post Thanks / Like
    Likes (Given)
    208
    Likes (Received)
    296

    Default

    10 IPM is only .0002" per flute, any 1/32 worth it's salt should be able to handle at least that. Watch your entry feed, most of the 1/32s I blow up are on the entries not the engraving itself.

  3. #3
    Join Date
    May 2012
    Location
    Mid-Iowa, USA
    Posts
    3,510
    Post Thanks / Like
    Likes (Given)
    3401
    Likes (Received)
    2032

    Default

    Whoops, it's a 2-fluter. 4.8IPM is .0002"/flute.

  4. #4
    Join Date
    Sep 2005
    Location
    South Carolina USA
    Posts
    4,397
    Post Thanks / Like
    Likes (Given)
    2049
    Likes (Received)
    1245

    Default

    Not sure of your part specs, but the Micro 100 engraving tools sure work well.. I just finished up some tiny numbers engraved on hard S-7 at 55 RC.

  5. #5
    Join Date
    May 2012
    Location
    Mid-Iowa, USA
    Posts
    3,510
    Post Thanks / Like
    Likes (Given)
    3401
    Likes (Received)
    2032

    Default

    Quote Originally Posted by Davis In SC View Post
    Not sure of your part specs, but the Micro 100 engraving tools sure work well.. I just finished up some tiny numbers engraved on hard S-7 at 55 RC.
    Gotta happen tonight. Only learned of the job last night (relatively typical around here) and it's cosmetic lettering. Nothing horribly special, but has to look good. I have two cutters to play with. That means I won't break one, right?

  6. Likes Mtndew liked this post
  7. #6
    Join Date
    Dec 2014
    Country
    CANADA
    State/Province
    British Columbia
    Posts
    621
    Post Thanks / Like
    Likes (Given)
    208
    Likes (Received)
    296

    Default

    Normal engraving for me is 10k and 10 IPM with a 4 flute (.00025 ipt) so if those two extra inches matter for quantity...

    Edit: looks like it's a onesie-twosie.

  8. Likes dstryr liked this post
  9. #7
    Join Date
    Jan 2010
    Location
    Gilroy CA
    Posts
    4,038
    Post Thanks / Like
    Likes (Given)
    2754
    Likes (Received)
    2081

    Default

    I used to always use a ball endmill but recently I've been using a #1 carbide center drill and been very happy with the results.
    #1 carbide about .003-.004 deep and you can really go fast.

  10. Likes Hertz liked this post
  11. Default

    Why .010 deep with a 1/32? Why not .005 with a 1/16 and triple your feedrate?

  12. Likes dstryr, chip_maker liked this post
  13. #9
    Join Date
    Sep 2007
    Location
    Northern VA
    Posts
    460
    Post Thanks / Like
    Likes (Given)
    4
    Likes (Received)
    53

    Default

    That sounds deep to me as well. I end up going only a few thou deep to get a pretty decent width line. Sneak up on it, and either ramp in or slow down the plunge like Haazart said.

  14. #10
    Join Date
    May 2012
    Location
    Mid-Iowa, USA
    Posts
    3,510
    Post Thanks / Like
    Likes (Given)
    3401
    Likes (Received)
    2032

    Default

    Quote Originally Posted by Hazzert View Post
    Normal engraving for me is 10k and 10 IPM with a 4 flute (.00025 ipt) so if those two extra inches matter for quantity...

    Edit: looks like it's a onesie-twosie.
    Just a onesie.

    Quote Originally Posted by dstryr View Post
    I used to always use a ball endmill but recently I've been using a #1 carbide center drill and been very happy with the results.
    #1 carbide about .003-.004 deep and you can really go fast.
    Don't have any of those.

    Quote Originally Posted by [email protected] View Post
    Why .010 deep with a 1/32? Why not .005 with a 1/16 and triple your feedrate?
    I can do that too, but then work will have to buy me a new one (not that that's a problem).

    Quote Originally Posted by Nami View Post
    That sounds deep to me as well. I end up going only a few thou deep to get a pretty decent width line. Sneak up on it, and either ramp in or slow down the plunge like Haazart said.
    Plunge right now is set to ~1.4 IPM.

  15. #11
    Join Date
    Feb 2012
    Country
    CANADA
    State/Province
    Ontario
    Posts
    1,043
    Post Thanks / Like
    Likes (Given)
    80
    Likes (Received)
    365

    Default

    Just ran the numbers and was going to lambast you for going so deep, but others have done it for me.

    HSMAdvisor would probably suggest higher feed and lower depth of cut.

    IMO. 0.01" deep with a 0.03" tool in 304SS is way too deep. Hence it suggests such a low feedrate.

    Otherwise you would probably snap the cutter right away.

  16. #12
    Join Date
    Jun 2006
    Location
    Thunder Bay Canada
    Posts
    1,658
    Post Thanks / Like
    Likes (Given)
    415
    Likes (Received)
    254

    Default

    I found that 0.003 to 0.004 was adequate for engraving with a 1/32 mill. The trick is that the surface has to be dead flat for such a shallow cut otherwise the letter widths will be all over the place.

  17. Likes Davis In SC, John Welden liked this post
  18. #13
    Join Date
    May 2012
    Location
    Mid-Iowa, USA
    Posts
    3,510
    Post Thanks / Like
    Likes (Given)
    3401
    Likes (Received)
    2032

    Default

    I'm going to change it to .005" with a 1/16" cutter. This is going straight on the subplate, so if it varies I'm going to blame Chick Workholding. Which I wouldn't mind doing anyway

    Edit: got the part indicated with a tenths test indicator (I have a VERY short flat to work with) within two tenths end to end, and checked the flatness of the part. Around the area to be engraved it's all within five tenths. Should work okay.

  19. #14
    Join Date
    May 2012
    Location
    Mid-Iowa, USA
    Posts
    3,510
    Post Thanks / Like
    Likes (Given)
    3401
    Likes (Received)
    2032

    Default

    Wish I could take a photo to show, but it came out awesome. 12k, 10.7 IPM, .005" deep.

  20. Likes Mtndew, zero_divide, Hertz liked this post
  21. #15
    Join Date
    Feb 2012
    Country
    CANADA
    State/Province
    Ontario
    Posts
    1,043
    Post Thanks / Like
    Likes (Given)
    80
    Likes (Received)
    365

    Default

    Quote Originally Posted by Atomkinder View Post
    Wish I could take a photo to show, but it came out awesome. 12k, 10.7 IPM, .005" deep.
    What do you know!
    That's exactly what my calc suggests for a 1/16 ballnose

    Thank for coming back with the results.

  22. Likes Atomkinder, Mtndew liked this post
  23. #16
    Join Date
    Jun 2012
    Country
    UNITED STATES
    State/Province
    Michigan
    Posts
    7,120
    Post Thanks / Like
    Likes (Given)
    2135
    Likes (Received)
    2315

    Default

    Don't know if this is related to OP but I see some software that claims to be able to use a JPeg ( photo the make the program. ) Is the true and easy?

  24. #17
    Join Date
    Nov 2011
    Location
    Missouri, USA
    Posts
    2,782
    Post Thanks / Like
    Likes (Given)
    1353
    Likes (Received)
    2703

    Default

    We regularly do deeper engraving @ 0.015 deep so it shows up after being painted, and sometimes even deeper so we can paint it, then fill in the remaining volume with a lacquer stick or contrasting paint.

    Looking at the last few we did, depending on situation, it was .003 - .005 depth per cut down to .015 depth, .0002" per tooth, and ~5ipm @ 10k rpm. That's with a 1/32 ball mill as well. The strategy might be 'playing it safe' but it's also a "onesie, twosie" where it had about $30k in each part before the engraving. Risk assessment resulted in taking it a little easy on the engraving with a 1/32 ball mill - acceptable time cost.

    ETA: Whoops, missed your followup post. Glad you had good success.

  25. Likes Atomkinder liked this post
  26. #18
    Join Date
    May 2012
    Location
    Mid-Iowa, USA
    Posts
    3,510
    Post Thanks / Like
    Likes (Given)
    3401
    Likes (Received)
    2032

    Default

    I'm here at work on my day off doing a different version because the engraving came out so nicely, so they're paying me OT to make them now.

  27. Likes John Welden, Mark Rand liked this post
  28. #19
    Join Date
    Aug 2011
    Location
    Toledo, Ohio
    Posts
    1,629
    Post Thanks / Like
    Likes (Given)
    38
    Likes (Received)
    556

    Default

    Quote Originally Posted by Atomkinder View Post
    I'm here at work on my day off doing a different version because the engraving came out so nicely, so they're paying me OT to make them now.
    .125 Spot Drills 90 do some awesome logos/engraving. I have the operator a firm believer

  29. #20
    Join Date
    Feb 2013
    Location
    Madison, WI
    Posts
    464
    Post Thanks / Like
    Likes (Given)
    748
    Likes (Received)
    274

    Default

    I have had the best luck engraving with drill mills.


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
  •