Announcement

Collapse
No announcement yet.

Engraving tool - D bit vs .. Dremel tool?

Collapse
X
 
  • Filter
  • Time
  • Show
Clear All
new posts

  • Engraving tool - D bit vs .. Dremel tool?

    Howdy gang. quick question for any of you out there that have done any engraving.
    In this case I'd like to try engraving using my CNC router .. so 20k rpm top speed, material to engrave is bronze.

    My instinct is to make a single lip 'd bit' style engraver.. perhaps 30* tip angle -- out of an old broken tap perhaps.

    When I got to wondering if I couldn't just use a dremel tool.

    I've got a small selection, among which is a very small 45* pointed tool.. maybe 6-8 flutes on it. Body diameter
    might be 0.1" or so and tapers to a point.

    I'd like to engrave graduations on the adjustment screw of a boring head I'm working on.. so the lines, preferably,
    would be mighty fine.

    Any advantage to one over the other? Or is there a better tool to do this job?

    Also, I'm way open to feedrate suggestions. I assume rpm for these tools is in the millions.

    Thanks!
    VS

  • #2
    Ah! Engraving, a topic that I realy like

    I have three preferences for engraving:
    -Small ball endmill, carbide, 2 Flute: Works very good on all materials, even hardened steel and is super durable.
    -"classic" D-Bit engraving bit: Easy to grind/resharpen, can produce a nice, fine line but the tip is a bit sensitive
    - Pyramid shaped engraving bit: Very uncommon, produces very vine engravings, very durable, easy to make. Works only in hard materials (steel/hardened steel). These are just a piece of round carbide (broken endmill..), ground to a three sided pyramid with 60..90° included angle on the tip.
    Here is a picture of the pyramid shaped bit:


    And a engraving done with it - The lines are 2/10mm apart, done on my manual engraving machine:


    I would not bother with HSS engraving bits anymore, carbide is the way to go.

    I engrave on the Cnc usualy at 20000rpm and 750mm/min (150mm plunge)
    Personal website

    Comment


    • #3
      Thanks Stefan -- that's a lot of options -- what do you suggest for bronze, carbide D bit? My guess is that the point would be tougher in HSS, no?

      Also, are you suggesting to not even try the dremel bit?

      Comment


      • #4
        If you have one, a small ball endmill would be my preference in soft material like bronze - 0,6mm would do the trick. If not, go for a D-Bit. maybe 60° included angle on the tip.

        And make sure you break the tip of the cutter slightly with a fine stone, but in respect to the clearance angles - Like this:


        In bronze HSS/carbide wont matter much.

        The dremel bit doesnt look like it realy has a cutting edge on its tip, I think it would produce a quite burry result, but you never know
        Last edited by stefang; 06-07-2016, 03:26 PM.
        Personal website

        Comment


        • #5
          The "D" bit because it is easy to make and sharpen. When durability is a concern, I have had success with the triangular bit Stefang pictures.

          Jim

          Comment


          • #6
            A small 2 flute 90 degree endmill works nicely, 1/8" or so. I use the D bits fairly often, the 60 degree ones with a .1 mm flat on the end. You can get 10 of those from China for way cheap on eBay. The 3 corner ones work well too.
            Kansas City area

            Comment


            • #7
              Sounds like experimentation time.. but those are some good leads, thank you.

              My markings are radial (boring head adjustment screw). Line spacing is probably from 0.4 - 0.6 mm (~0.020" on average).

              I'm shooting for 100 division on a 3/4" face -- the CNC will do it, but I don't know if I'll be able to read it when its done.

              Failing that, I'll go to 50 divisions.

              Stefan.. those 0.2mm spaced lines look gorgeous.

              Comment


              • #8
                I have done a bit of engraving during my years of employment and we always used single edged cutters with a small flat (.007/.012) stoned on the tip, the flat should have clearance in both directions, use some type of cutting oil. Also we always used Silly Putty to check the depth and shape of the lettering, remove all the burrs and oil first, press it in remove it to see what it looks like. I do not think Dremel Tools run very concentric probably because of the cheesey collet they have.

                frankie

                Comment


                • #9
                  ok! not perfect, but better than I expected for a first-time CNC engraving.

                  100 divisions on a 3/4" face.

                  Pictures below.

                  Used an HSS D-bit, 60* included angle. By the looks of it, it could've been sharper.. pushed up a bit of a burr.

                  The 4 and 7 are missing some lines, but that was likely my fault in the CAM.

                  I expect I could hit this with emery to clean up the burrs?

                  My plan was to fill the engraving with black wax, but the lines are surprisingly legible.

                  The hex was also cut in the CNC.



                  Comment


                  • #10
                    Looks already good, I would chuck it up in the lathe and hit it with a fine file

                    I fill most of my engraved dials just with black felt pen and rub the overpaint off with some common copy paper.

                    Ps: That scale would drive me crazy.
                    Personal website

                    Comment


                    • #11
                      The screw is 1mm pitch, the scale is 1/10 mm on the numbered divisions. 1/100 of course on the fine.

                      I don't think I would've had the room to number 0-100

                      Suggestions for next time?

                      Comment


                      • #12
                        Not exactly what you're doing, but I thought I throw these out there for general consumption.

                        I've used the 60 and 90 degree end mills in aluminum too. Filled with paint and 'brushed' off the excess with the belt sander:



                        And I built a scratch engraver. Turned, drilled and reamed the body 1/16", a bit of drill rod, half an ink pen spring, and a couple of drops of JB Weld. I'd like to make another with carbide instead of drill rod:
                        Edit - It's held in the spindle, but I don't turn the motor on.



                        I engrave wine keys and bottle openers for my friends. Basically just scratching off the powder coat:

                        Definition: Racecar - a device that turns money into noise.

                        Comment


                        • #13
                          Thats some nice work!

                          Question jumps to mind: scratch/drag engraving vs. cutting -- when to use one over the other?

                          Comment


                          • #14
                            The burrs can be a pain because they will often just fold back into the engraving on cleanup. What I usually do is once the final depth has been hit, I use a fine stone to smooth things and then run the program again. This cleans out any pushed-over burrs. Obviously done before pulling from the machine!
                            George
                            Traverse City, MI

                            Comment


                            • #15
                              Getting back to the idea of the Dremel tool. I'm sort of thinking that since you'd be working only with the very tip where the flutes are not very deep or even well formed that chip clearance would be nasty. I suspect that a D bit with the correctly done micro beveled end stoning as shown above would be a better way to go.
                              Chilliwack BC, Canada

                              Comment

                              Working...
                              X