Chamfer Mill for Engraving
Close
Login to Your Account
Results 1 to 12 of 12
  1. #1
    Join Date
    Dec 2017
    Country
    UNITED STATES
    State/Province
    North Carolina
    Posts
    37
    Post Thanks / Like
    Likes (Given)
    18
    Likes (Received)
    3

    Default Chamfer Mill for Engraving

    Good evening and Happy New Years!!!
    I am trying to set up engraving on Autodesk Inventor. I was told that its best to use a Chamfer tool for this operation. My question is, What size tool and how should I set this up? Many thanks in advance!!!!

  2. #2
    Join Date
    Sep 2005
    Location
    Oakland, CA
    Posts
    1,936
    Post Thanks / Like
    Likes (Given)
    58
    Likes (Received)
    437

    Default

    I've always had good luck using very small combined center drills. Depends on how wide a line you want.
    I engrave .300 high letters with a depth of cut of about .003".

  3. Likes Booze Daily liked this post
  4. #3
    Join Date
    Apr 2015
    Country
    UNITED STATES
    State/Province
    Connecticut
    Posts
    214
    Post Thanks / Like
    Likes (Given)
    126
    Likes (Received)
    97

    Default

    I’ve found a nice sharp drill/Mill does the trick and you can get them at 60* included. I would also second a center drill if your in a pinch or don’t have the means to get another tool.

  5. #4
    Join Date
    Dec 2014
    Country
    UNITED STATES
    State/Province
    Washington
    Posts
    62
    Post Thanks / Like
    Likes (Given)
    99
    Likes (Received)
    20

    Default

    Are you asking how to set this up in inventor or suggestions on what tool to physically use?

    For the CAM side of things, just tell it no cutter comp and it doesn't matter what you load in the spindle. Your verify will look different so you may prefer to have that accurately represent what you are using.

    For tool suggestions we religiously use 1/32 ball mills (robjack, Harvey, accupro) and they come out beautiful. very strong tools.

  6. #5
    Join Date
    Dec 2017
    Country
    UNITED STATES
    State/Province
    North Carolina
    Posts
    37
    Post Thanks / Like
    Likes (Given)
    18
    Likes (Received)
    3

    Default

    Quote Originally Posted by BSCustoms View Post
    Are you asking how to set this up in inventor or suggestions on what tool to physically use?

    For the CAM side of things, just tell it no cutter comp and it doesn't matter what you load in the spindle. Your verify will look different so you may prefer to have that accurately represent what you are using.

    For tool suggestions we religiously use 1/32 ball mills (robjack, Harvey, accupro) and they come out beautiful. very strong tools.
    Will the ball mill produce a square engraving? Also, someone had mentioned something about pocket milling. Would that be something I could do?

  7. #6
    Join Date
    Sep 2007
    Location
    Northern Illinois
    Posts
    3,090
    Post Thanks / Like
    Likes (Given)
    1365
    Likes (Received)
    1596

    Default

    Quote Originally Posted by cmmpro1 View Post
    Will the ball mill produce a square engraving? Also, someone had mentioned something about pocket milling. Would that be something I could do?
    No, it will give you a semi-circular groove for the letter stroke, unless you go deeper than half the diameter of the tool.

    For engraving to look crisp, it needs to have sharp corners. The different suggested chamfer mills and spot drills may do that, but because they come to a sharp point, that point will wear quickly and become rounded, leaving a radius at the bottom of the V groove. Obviously less of a problem in aluminium than in hardened steel.

    The traditional tool for engraving is a single lip cutter with rather steep sides and a flat tip. This makes a groove that looks square, with a flat floor. Here is a link to the tool:
    Series 37- | .5" Tip Solid Carbide One Flute Straight Engraving Bit w / 6 Degree Angle (Item 37-1) | Item Detail | LMT Onsrud

    The "degree angle" is the included angle; each side is half that. The "tip" diameter is the width of the flat it puts at the bottom of the groove. I've run these in S-7 and A-2 steel hardened to Rc 56-59, with good luck, anthough they certainly last longer in softer material.

    Dennis

  8. Likes cmmpro1, Pathogen liked this post
  9. #7
    Join Date
    Sep 2007
    Location
    Northern Illinois
    Posts
    3,090
    Post Thanks / Like
    Likes (Given)
    1365
    Likes (Received)
    1596

    Default

    Duplicate post.

  10. #8
    Join Date
    Dec 2017
    Country
    UNITED STATES
    State/Province
    North Carolina
    Posts
    37
    Post Thanks / Like
    Likes (Given)
    18
    Likes (Received)
    3

    Default

    Quote Originally Posted by Modelman View Post
    No, it will give you a semi-circular groove for the letter stroke, unless you go deeper than half the diameter of the tool.

    For engraving to look crisp, it needs to have sharp corners. The different suggested chamfer mills and spot drills may do that, but because they come to a sharp point, that point will wear quickly and become rounded, leaving a radius at the bottom of the V groove. Obviously less of a problem in aluminium than in hardened steel.

    The traditional tool for engraving is a single lip cutter with rather steep sides and a flat tip. This makes a groove that looks square, with a flat floor. Here is a link to the tool:
    Series 37- | .5" Tip Solid Carbide One Flute Straight Engraving Bit w / 6 Degree Angle (Item 37-1) | Item Detail | LMT Onsrud

    The "degree angle" is the included angle; each side is half that. The "tip" diameter is the width of the flat it puts at the bottom of the groove. I've run these in S-7 and A-2 steel hardened to Rc 56-59, with good luck, anthough they certainly last longer in softer material.

    Dennis
    AWESOME!!!!! Thank you for the information and the link!!!

  11. #9
    Join Date
    Jun 2012
    Location
    Michigan
    Posts
    3,491
    Post Thanks / Like
    Likes (Given)
    2859
    Likes (Received)
    2023

    Default

    Have a look at these, they are really nice and leave a crisp line.
    HIGH PERFORMANCE ENGRAVING END MILLS

  12. Likes Pathogen liked this post
  13. #10
    Join Date
    Mar 2013
    Country
    UNITED STATES
    State/Province
    Oregon
    Posts
    1,131
    Post Thanks / Like
    Likes (Given)
    476
    Likes (Received)
    1180

    Default

    Quote Originally Posted by Mtndew View Post
    Have a look at these, they are really nice and leave a crisp line.
    HIGH PERFORMANCE ENGRAVING END MILLS
    I was going to suggest these as well. I just ordered one, but I've heard very good things about them.

    I'm currently running a Nine 9 inserted engraver. It's a very trick tool, but it's essentially a single flute cutter and it runs kinda slow (12ipm in aluminum, and that is sorta pushing it). The Lakeshore can be run at 20ipm @ 10k. I have one part that has about 60 seconds of engraving bullshit on it, and this should nearly cut my cycle time by 20 seconds or so.

  14. Likes Mtndew liked this post
  15. #11
    Join Date
    Sep 2007
    Location
    Northern Illinois
    Posts
    3,090
    Post Thanks / Like
    Likes (Given)
    1365
    Likes (Received)
    1596

    Default

    The OP hasn't told us what material he needs to engrave, or how hard it is, or how deep he needs to go. The Lakeshore cutters have ball noses, but steeper sides, and being two flute, should run faster, The Ostrund cutters I linked cut a flat bottom groove, which does me better because I engrave inventory numbers on the back of mold inserts, and I do it before heat treat and final grinding (usually). I typically engrave .012" deep with a nominal .007 grind allowance, and hope I end up with engraving between .003" and .008" deep. The .003 would be into the round bottom, and the engraving would look wimpy, while with a .020" wide flat bottom, it's still OK if it's only .002" deep.

    Different situations point to different tools, but all these taper tools are considerably stouter than say, a .020" ball nose end mill. The OP will have to try one of each and see which effect suits him best.

    Dennis

  16. #12
    Join Date
    Dec 2017
    Country
    UNITED STATES
    State/Province
    North Carolina
    Posts
    37
    Post Thanks / Like
    Likes (Given)
    18
    Likes (Received)
    3

    Default

    Quote Originally Posted by Modelman View Post
    The OP hasn't told us what material he needs to engrave, or how hard it is, or how deep he needs to go. The Lakeshore cutters have ball noses, but steeper sides, and being two flute, should run faster, The Ostrund cutters I linked cut a flat bottom groove, which does me better because I engrave inventory numbers on the back of mold inserts, and I do it before heat treat and final grinding (usually). I typically engrave .012" deep with a nominal .007 grind allowance, and hope I end up with engraving between .003" and .008" deep. The .003 would be into the round bottom, and the engraving would look wimpy, while with a .020" wide flat bottom, it's still OK if it's only .002" deep.

    Different situations point to different tools, but all these taper tools are considerably stouter than say, a .020" ball nose end mill. The OP will have to try one of each and see which effect suits him best.

    Dennis
    Thank you for the information!!!!


    Sent from my iPhone using Tapatalk Pro


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
  •