Announcement

Collapse
No announcement yet.

More CNC Questions

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

  • More CNC Questions

    1) How do you establish the relationship between the cutter and the work? Do you have to "just touch" the work with the cutter and hit a zero button? In all 3 planes (on a miller, 2 on a lathe)? Every time you change cutters?

    2) Am I right that CNC lathes can cut threads without using a gear train to control the leadscrew? If so, and the leadscrew is controlled by a stepper or servo motor, how do the electronics calculate how to move the motor? I'm assuming there is some type of encoder on the spindle that generates, say, 1024 pulses per spindle rotation. But no matter what the number of pulses per revolution, most screw pitches won't divide into it evenly. Seems as if it would take some fancy footwork to avoid pitch errors, especially if you have to calculate all this stuff while the spindle is turning. Or is there some simple method I have missed?

  • #2
    On a CnC lathe, typically tool #1 is always your reference tool, so the offsets should be zero on the x and z...once you found the right numbers with your tool 1, then all your other tools you will need to touch each one off the x and z so you can input your offsets...

    On a Mill, the x and y are always the centerline of your tool, so you only need to reference your z on each tool, your x and y will always be the same on each tool because it is centerline.. For referencing your z on your tools, all you need to do is touch each tool on a surface that usually is your zero...Different machines use slightly different techniques...You can probe each tool, but some probes are expensive, so All I do is just use a piece of paper to touch off the tools.....

    hope this helps

    brent

    Comment


    • #3
      CNC controls look at the relationship between the "home" position and the arbitrary "zero" that the operator establishes. This applies to your tool offsets as well as your part zero. The values that you set for any zero point are typically the absolute distances from the home position to the point in the work envelope you establish as zero. Most turning centers now have auto. tool probes for measuring the tool offsets. You simply touch the tool to the probe and the number is entered into the corresponding tool offset number. Machining centers have these features but they are usually sold as options on the machine and can interfere with the amount of work space and are expensive. Many of the machining centers will allow you to jog to the place that will be zero and set by pushing a button. FADAL machining centers for example have the tool setting cycle. The operator jogs the tool to the top of the part(or whatever point you want as zero) and touches each tool used for the job. Once you push the button it stores the value and loads the next tool and the process is repeated for all tools you need.

      Thread cutting on all new machines with conversational controls is as simple as telling the control where in z to start the thread and what pitch you are cutting and the major diameter. Sometimes you may have to enter the thread depth which can be calculated or looked up in the handbook. The machine uses a code I think it is G33 to syncronize the turret and spindle. Set your rpm and feed rate in inches per minute or set constant suface footage and inches per rev to give proper pitch. Pitch as you know is 1/threads per inch. Feed in inches per minute is rpm x pitch. I would say that most any machine will have a canned threading cycle to figure the depth of cut per pass and the infeed angle if not, you have to do the math.

      Hope this helps.I don't type fast so I try and condense my answers. If you are confused please advise and I will try and clarify.

      CT

      Comment


      • #4
        Lathe spindles have an encoder. An encoder uses revolutions or a wheel behind the spindle that sends pulses back to the control. here is an example. One lathe I have has a 6 inch plate behind the spindle with holes at 6 degree increments. The plate spins like the spindle, and a "pick-up" senses each hole as it passes by the pick-up. The holes are 1/8 inch in from the edge. One hole is actually a notch to the edge of the plate. a second pick-up uses this notch only. This notch starts the thread in the same place each time. For a multi pitch thread, the notch is found, and the number of holes from this notch are determined. The encoder works much on the same principle, as the start of the thread is set where the beginning of one revolution of the encoder is determined.

        This is just based on two lathes I use.

        CCBW, MAH

        Comment


        • #5
          Brent;I think you may have left out that the mill needs to be told the diameter of the cutter. In larger machine shops they may have a tool presetter. The mill or lathe tool will be installed in a tool holder which is then measured. A list is generated and then the operator will enter the tool dimensions into the tool list.
          Bill

          Comment


          • #6
            OK, I think I understnad about setting zeros for tool position.

            Now let's get down to brass tacks on the threading question. Let's say that instead of building a gearbox for my 6" Atlas lathe, I want to put an encoder on the spindle and a stepper on the leadscrew and cut threads that way.

            Assume a 6 degree encoder (60 pulses/rotation). Assume a 200 step per revolution stepper. The 6" Atlas has a 16 TPI leadscrew. Assume I want to cut a 14 TPI thread.

            I need 16 leadscrew revolutions for every 14 spindle revolutions. Therefore I need:

            16 x 200 steps for 14 x 60 pulses, or
            1 step for every 0.2625 pulses.

            How do you accomplish that, or any other screw pitch that doesn't correspond to an integral number of pulses? (BTW, in this example, 1 step/pulse gives 53 1/3 TPI - not too useful.)

            Comment


            • #7
              alsinaj:
              Professional machines use quality encoders. Glass scales are preffered. Some encoders output 30K+ pulses per revolution. Many commercial machines these days have ball screws that are 4 or 5 TPI to allow high speed rapids.

              What you are describing was done by two European gentlemen for their hobby lathes. They got rid of the gear change box and drove the leadscrew directly for both feed and threading. Threading is the most difficult because the crosslide position is calculated for each angular position of the lathe spindle. Could be done - and done quite well. Those two gentlemen's worked but needed "tweaking".



              Comment


              • #8
                I can't address the use of servo motors, but if you're thinking of using a stepper, there are several possibilities.

                1. Drive the spindle with another stepper motor. Then you can pulse the spindle motor and the leadscrew motor in whatever arbitrary pattern you like.

                2. Use a clock frequency high enough so that both pulse rates are integral tick counts. In your example, the ratio of encoder pulses to stepper pulses is 21:80, so if we could generate a clock 80 times encoder pulse rate, we could pulse the leadscrew motor once for every 21 pulses of the derived clock. In the real world, rather than generating a different clock for every TPI, you would probably use a 1KHz clock, calculate the spindle RPM from the encoder output, and calculate the stepper motor pulse intervals to the nearest millisecond.

                3. If you want to let the spindle encoder pulses drive the process, you can dither the pulse rate to the leadscrew motor. At each input pulse, calculate the correct number of leadscrew pulses and round it to the nearest integer. Using your example, the first 30 steps would be

                4 4 3 4 4 4 4 3 4 4 4 4 4 3 4 4 4 4 3 4 4 4 4 3 4

                Pulsing the leadscrew motor four times for every spindle pulse seems like it would generate kind of a wavy thread. The threading tool would always be getting behind and jumping to catch up. Given the inertia and slop in the physical setup, and the realities of stepper motor timing, it's probably not that bad. But if you like, you can make it a lot smoother by increasing the resolution on the encoder. If you put a 200 step encoder on the spindle and stay with a 200 step motor on the leadscrew, then you'd be pulsing the leadscrew motor once for every encoder pulse plus one extra on every seventh encoder pulse.

                Comment


                • #9
                  Here's a crack at motivating the leadscrew on homebrew CNC lathe: Use a 2mm pitch leadscrew, 200 step/revolution motor on the leadscrew, and a 127 pulse/revolution encoder on the spindle. For imperial threads, multiply the spindle encoder pulses by 40, divide the resulting pulse train by twice the desired TPI, and use resulting pulses to drive the stepper. For metric threads, multiply the spindle encoder pulses by 10 x the desired thread pitch in mm, divide the resulting pulse train by 127, and feed the resulting pulses to the stepper. No approximations, no error. Other metric leadscrew pitches can be used, with appropriate adjustments to the multiply/divide coefficients.

                  The "multiply" process could be a problem. The only way I know to multiply a pulse train by an arbitrary integer is to use a phase-locked loop with a divider in the feedback loop. That way, you can multiply by dividing (like bacteria). The tricky part is achieving and maintaining lock. But for threading, there should not be any rapid changes in spindle rpm, so it might not be so tough. Comments?

                  Comment


                  • #10
                    Oops! The above should read "For metric threads, multiply the spindle encoder pulses by 100 (not 10) x the desired thread pitch in mm," etc.

                    Comment


                    • #11
                      Hey bill neulfild,, You are right about the diameters on the mills, what i meant was that all you have to do is set the offset for z, all your diameters can be inputed later when convenient..you don't have to touch off each tool on the diameters, just the length...

                      sorry for not being more detailed

                      brent

                      Comment

                      Working...
                      X