Page 1 of 2 12 LastLast
Results 1 to 15 of 23

Thread: Some CNC work....

  1. #1

    Some CNC work....

    This is a tapered spiral with a twist, not a straight taper. The flute radius varies down the taper (not done with a pattern router bit).

    Hand coded and run on a M400 Centroid control using the macro language. Relatively short program with the cutter path calculated on the fly, less than 50 lines of Gcode. Blank was held in the 4th axis, sharp vee tip wheel cutter cutting on the side of the blank (as opposed to on the top).
    Attached Images Attached Images

  2. #2
    Pyrography.

    Again 4th axis on the round parts.

    The burning is done either with a soldering iron mounted on my machine's quill or with a 3 watt diode laser likewise mounted. The laser is more forgiving on "depth" of cut, but diode lasers are dangerous. I've found conventional wood burning tools, even the high end variety, don't work well in this application. They get very hot and also cool very quickly when they're fed into the work leaving an initial dark impression which tapers off due to the tips cooling. My digital soldering iron maintains constant tip temperature, only 850 degrees F though which means slow feed rate.

    Note the ukibori on the second to right piece's lower end.
    Attached Images Attached Images

  3. #3
    Unicorns..?

    These are done with the part standing upright. A wheel cutter moves downward in the arc paths. Then the part is rotates one degree or so and the cut is repeated dropping the starting point in Z down 1/360th of the pitch.

    A very short program, again programmed in Centroid macro language.
    Attached Images Attached Images

  4. #4
    Spiral with variable pitch, 8 flutes. Part is held in the 4th axis.
    Attached Images Attached Images

  5. #5
    Domed end on work.
    Attached Images Attached Images
    Last edited by Doug Rasmussen; 06-02-2016 at 11:03 PM.

  6. #6
    Some metal work. An alunimum die to press a flower design in copper sheet. Work piece is flat on table.
    Attached Images Attached Images

  7. #7
    Join Date
    Feb 2003
    Location
    In the foothills of the Sandia Mountains
    Posts
    14,953
    Very impressive Doug. Are you G coding all of this by hand?
    What kind of cnc are you running?
    Please help support the Creek.

    My mechanic told me, "I couldn't repair your brakes, so I made your horn louder."

    - Steven Wright

  8. #8
    Quote Originally Posted by Bruce Page View Post
    Very impressive Doug. Are you G coding all of this by hand?
    What kind of cnc are you running?
    Thank you Bruce.

    Yes it is mostly hand coded. There might be a small segment of CAM code. For instance, the spiral pieces. there would be a few lines of code to generate the arc for a single flute. then you repeat that say 6 times around the workpiece for a six flute spiral. then you step lengthwise down the blank using the control's scale function to resize the flute giving a taper. Basically, you take a simple cut, repeat, scale it, repeat and so on and so on.

    My control is a Centroid, a fairly powerful control that allows you to do things in Gcode that sometimes are easier to program than to draw. The machine is a basic knee mill with 4th axis. It's a bit larger than a Bridgeport.

    As a simple example. With a basic arc command, G02, you could route a circle. Then you could tell the control to repeat the circle but at 80% of original size. Keep repeating the circle at less size and you would end up with a series of concentric circles only having programmed one circle.

  9. #9
    Way, way cool.

    For anyone using the limited G-code set which Grbl supports, there’s now a pre-processor which extends that to support most of what LinuxCNC supports: https://github.com/NRSoft/GSharp — looking forward to seeing it built into every G-code sender.

  10. #10
    Did you CNC the Ukibori or is it conventional?

    +1, nice work
    Sometimes I just want to look at pretty pictures,... Thats when I go to the Turners Forum

  11. #11
    Join Date
    Oct 2006
    Location
    Bloomington, IL
    Posts
    5,933
    I too have centroid with a 4th axis - mine is on a knee mill I retrofitted with an allinonedc. Would you post the gcode so I could see it and try and understand it. I am new to the 4th axis setup on mine. miek at thewoodworker dot net is my hiom eemail if it is easier just to email it.

    Very awesome work.
    Glad its my shop I am responsible for - I only have to make me happy.

  12. #12
    Quote Originally Posted by Mark Bolton View Post
    Did you CNC the Ukibori or is it conventional?

    +1, nice work
    Yes, it was done with the CNC. A small diameter jewelers dapping punch was used as the tool. The dapping punch was held in a collet like a router bit to make the impression in the work. A skim cut with a router bit was done, then steaming to raise the pattern.

  13. #13
    Quote Originally Posted by Mike Heidrick View Post
    I too have centroid with a 4th axis - mine is on a knee mill I retrofitted with an allinonedc. Would you post the gcode so I could see it and try and understand it. I am new to the 4th axis setup on mine. miek at thewoodworker dot net is my hiom eemail if it is easier just to email it.

    Very awesome work.
    IMO, the most complicated part of 4th axis work is calculation of a rotary feed rate equivalent to the feed rate used in normal 3 axis work where the feed is expressed in inches per minute, ipm. When the 4th axis is used the feed rate has to be specified in degrees per minute.

    G01 X5 F20. This would be the way a non-rotary move might written. Feed at 20 IPM from the current position to X5.

    G01 A300 F1146. This is a rotary feed rate of 1146 degrees per minute on a 2" diameter piece equivalent to a non-rotary feed of 20 ipm. The feed rate is dependent on the work diameter.

    Let's do the math. 2" diameter has circumference of 6.28" At 20 ipm, 20/6.28=3.18 revolutions per minute. Multiply that by 360, and you get an equivalent rotary feed rate of 1146 degrees per minute.

    Anytime there's rotary axis feed it has to be in degrees per minute. But, there are controls that do the calculation internally so no need for the math. Unfortunately Centroid is not one of those controls.

    Things get worse when you have a combination of linear and rotary feeds like G01 X5 A300 F1000

    Here's a link to a formula to calculate combined feeds.
    http://www.cncsnw.com/4thHowTo.htm





  14. #14
    In my previous post about calculating rotary feed rates I left off with no easy solution to what can be complicated.

    I use Millwrite software to do the calculations. That makes it easy, Millwrite uses the flat pattern Gcode and wraps around the work of the diameter you specify.

    Cncsnw also offers a program to calculate the rotary feed rates.

    I have a spreadsheet setup to do it. It needs some work though, not quite ready for public consumption as it's a little cumbersome to format the
    Gcode for spreadsheet input.


    For a few years I've been trying to get some straight answers from Vectric whether their software will automatically calculate rotary feed rates. I had a few exchanges with Vectric tech support ending in them basically telling me I didn't know anything about CNC's. Recently an individual at Rockler told me the Vectric software had now been modified to calculate rotary feed rates, but apparently I've been put on Vectric's ignore list because they don't respond any more. Maybe someone on this forum can tell us how Vectric handles rotary feed rates currently.

  15. #15
    Maybe someone on this forum can tell us how Vectric handles rotary feed rates currently.
    The simple answer, is that they don't. At least not in the the program itself.

    For some machines, they have the post processor output lines of code that calculate the feedrate. The post processor has access to the "wrap diameter" info, and by using that and the feedrate, they output a formula that calculates the feedrate for a axis moves.
    I've never used this, and just took a quick look at the included shopbot and camaster posts that do this.
    Gerry

    JointCAM

Posting Permissions

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