Announcement

Collapse
No announcement yet.

Questions about CNC

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

  • Questions about CNC

    I have two questions about CNC machines?

    1. Do they all have DRO for close-loop control on all axis?

    2. How is the tool wear comepensation done? It is calculated or do some machines actually sense or measure the wear and compensate accordingly?

    Thanks.

    Albert

  • #2
    Albert,

    Don't know about the closed loop.

    The machine uses values that are stored as variables to claculate how much to offset the tool path when using TRC. These values have to be input into the control memory. They can be input by the operator or by using some type of probe or laser device. In all situations some measurement is made to determine the value needed. Most CNC turning centers now have tool probes for setting the tool offset values most machining centers can be set up with probes for measuring tool dia and height as well as probes for measuring the part being run. High end O.D. grinders can be fitted with a device that monitors the size of the part during the grinding process and makes the needed adjustments while the wheel is in contact with the part. You can add as an option on many machine tools a featur called tool load monitoring that will tell the machine to stop using a tool when the spindle load reaches a designated point. This feature prevents the use of dull tools and spindle overloads. Nearly all machines will allow the use of macro programming and probes to give the user the ability to measure or monitor anything.

    CT

    Comment


    • #3
      Albert,

      99.9% of cnc machines use servo motors which rotate the ballscrews thus moving the respective axis.

      Now don't get this mixed up with Servo which makes a kinda sorta CNC conversion for manual machines which takes it's positions from the DRO. Kinda a neat system, won't do all that a full servomotor cnc machine will do. I don't think it will do circular interpolation and such.

      Tool compensation.

      Tool comp is a term for a CNC funtion. For instance with a mill one can simply program the finish surface path, enter the tool diameter into tool chart in the machine controller and it will cut properly, or it's supposed to work this way. Don't get your G41 and G42 mixed up.

      Example cutting around a 1" x 2" square with a 1/2 endmill 1/2 tall or deep.

      No tool comp.

      M3 ---- starts spindle in clockwise rotation
      G0 x-.5 y-.25 z .5 Goes here in rapid
      G1 z-.5 f6 programed feed down
      x 2.25
      y 1.25
      x-.25
      y-.1 ...to get past corner
      G0 z.5 ...spindle pops up to 1/2 above
      M6 parks in home position

      with tool comp.

      T1M6 -- tells which tool from chart
      M3
      G0 x-.5 x 0 z .5
      G1 z-.5 f6
      g42 -- cutter to the right of part
      x 2
      y 1
      x 0
      y -.1
      G0 z .5
      M6

      This is just an example, see with cutter comp one doesn't have to allow for diameter of tool. If tool has been resharpened this can be compensated for in the tool table, also with some tweekin of tool comp numbers and or reverse comp. for leadscrews one can put finished part dead on.

      Controllers are getting more sophistocated, most new ones are PC based. Feedback from a CMM can be used to adjust tool comp. , some will adjust to a point then shut down and notify operator. Lights out machining is the goal anymore.

      This is my grasp on the situation. I'm not too high tech, hafta run an old CNC mill at work once in a while. I read the articles in the American Machinist and Modern Machine Shop and am amazed at the latest greatest technology.

      Oh yea, I have to do my own tool comp. numbers, as I said we aren't too sophisticated.

      Comment


      • #4
        When using tool comp imagine that you are walking the path that is programmed and right(G42) is your right and left (G41) is your left. Besure to turn off tool comp immediately after the path is complete and make sure cutter is at least 1/2 of it's diameter plus some away from anything you don't want cut. Tool comp is modal meaning it is on untill you turn it off. Imagine 3.5 dia face mill running with a .5 dia offset results could be disasterous.

        Comment


        • #5
          Some systems also detect tool dullness by monitoring the current drawn by the machine's motor. All else being equal, it takes more power to shove a dull tool through the work than a sharp one.

          Comment


          • #6
            Question #1 - CNC Machines usually run on an encoder loop. The machine moves a distance, and feedback betwen the control moved distance and actul moved distance is measured and double checked as the machine is moving and constant. This is for most machines. Some do not do "double checks" . The encoder checks the actual moved length. feedback loop. The machine measures "lag" throughout the move, and corrects for it.

            I have to set 6 controls in my shop, and the lag balance is the hardest thing to keep set. The control reads .0002 or less behind the actual move, thus the move is compensated in the actul move. Over .0002 lag on my machines, they shut down.

            also have three machines where the servos just move the table. I have to adjust "steps" to make this right. These are stepper motor machines. The number of steps in one inch is the ticket here, and this takes patience, and a very good one inch indicator.

            #2. Tool diameter. Most machines do NOT measure tool wer on their own. You put the actual tool diameter or radius on a chart (register) in the mahcine control. The machine looks up this chart, and uses your figure. You have to compensate this after you measure a part for closer correctness.

            The machine looks up info you provide. You make the adjustments. CNC machines are very stupid. They are totally dependent on the operator and programmer perhaps more than a common bridgeport. A common Bridgeport has the common instinct sense of the operator knowing that a cutter is not turned on, a cutter is dull, running backwards, or a part not clamped. A CNC machine will run a part completely through after it has thrown it from a vise or beaten the heck out of an improperly clamped part. It will try to cut a piece without a spindle on. It will tap a part before a hole is drilled. It will run thousands of parts undersized without knowing or caring. The operator is the brains, and must be aware that instinct is not an issue with CNC as much as awareness.
            CCBW, MAH

            Comment


            • #7
              Albert
              Any CNC machine with AC servos will have either a shaft encoder or glass scales giving actual feedback to the system. Steppers can be run with out encoders by counting steps. Problem with that is if the motor is undersized the work can over-run the motor past its stop position. Using feedback makes the most sense from an accuracy standpoint. The AC servos also have smoother torque, higher startup and running torque, and run cooler. They also cost a lot more.

              Some of the ISO 9001 shops up here have gone to daily checks of tooling with presetters & microscopes and the information is programmed into a Dallas chip installed in the shank. This information is read as the tool is selected and automagically compensated for. The one engine rebuild shop that did this has higher quality control and less rejects now. The owners bitched and moaned when they first started it - lots of money - but it has paid for itself just in reduced screwups. I am told now they think it was "their idea".

              Comment

              Working...
              X