Thread: Emco PC120 Turn

Page 3 of 12 FirstFirst 12345 ... LastLast
  1. #21
    Chaz's Avatar
    Lives in Ickenham, West London, United Kingdom. Last Activity: 7 Hours Ago Has been a member for 4-5 years. Has a total post count of 811. Received thanks 39 times, giving thanks to others 33 times.
    Quote Originally Posted by m_c View Post
    You have to use a dial gauge to get the drill on centre in the X-axis movement. Stick the dial gauge to the chuck, then spin the chuck/dial gauge around the shank of the drill/holder, and jog the X axis until the drill is on centre. If the drill is at the wrong height, then there's an alignment issue with the turret.

    If you have accurate homing, then you don't need a master tool. All the offsets are simply taken from the home position.
    The master tool process is only needed if you're homing the machine manually, so you can take a test cut with the master tool, then enter that value to manually set the machine position, then have all subsequent tool offsets set from the master tool.


    If the machine is running Mach3 via the parallel port, then to thread you need a single pulse. Originally there would likely of been some form of multiline sensor on the spindle, but it's of no use to the parallel port.
    Thanks. I tried to put on a dial gauge last night but space is an issue. I need a smaller setup.

    In terms of home position, I am hoping that with electrical proximity switches, this will be fairly accurate. I will do some tests later.

    On the sensor for the spindle, I noted what I recall to be 3 wires coming out from the sensor. Let's assume this is a single pulse (or needs to be converted somehow), is there normally an input into the BOB or similar to read these? If the sensor is damaged, is there a part that can be bought that will give me what I need (like a generic generator that works with most setups)?

    Many thanks for your help / info, been very useful.

  2. #22
    m_c's Avatar
    Lives in East Lothian, United Kingdom. Last Activity: 8 Hours Ago Has been a member for 8-9 years. Has a total post count of 1,661. Received thanks 174 times, giving thanks to others 5 times.
    Quote Originally Posted by Chaz View Post
    Thanks. Where / what determines the direction of spindle rotation per tool?
    Where the cutting edge is, and what direction the material has to turn in relation to the cutting edge. The turret on my lathe is rear mounted with the disc machined so 12mm tools have their cutting edge level and facing down when at the spindle (click the pic if you want to see a vid of it changing position a couple times)
    Avoiding the rubbish customer service from AluminiumWarehouse since July '13.

  3. #23
    Chaz's Avatar
    Lives in Ickenham, West London, United Kingdom. Last Activity: 7 Hours Ago Has been a member for 4-5 years. Has a total post count of 811. Received thanks 39 times, giving thanks to others 33 times.
    Quote Originally Posted by m_c View Post
    Where the cutting edge is, and what direction the material has to turn in relation to the cutting edge. The turret on my lathe is rear mounted with the disc machined so 12mm tools have their cutting edge level and facing down when at the spindle (click the pic if you want to see a vid of it changing position a couple times)
    Sorry, my question was unclear.

    I understand when I need CW and when CCW. What 'setting' tells the spindle to rotate CW or CCW depending on the tool choice?

  4. #24
    m_c's Avatar
    Lives in East Lothian, United Kingdom. Last Activity: 8 Hours Ago Has been a member for 8-9 years. Has a total post count of 1,661. Received thanks 174 times, giving thanks to others 5 times.
    Quote Originally Posted by Chaz View Post
    Sorry, my question was unclear.

    I understand when I need CW and when CCW. What 'setting' tells the spindle to rotate CW or CCW depending on the tool choice?
    There's not a setting for that. You'll need to ensure however you produce your G-code does the spindle direction setting.

    You could allocate blocks of tool numbers that rotate certain directions, then use the M6 macro to check and set spindle direction depending on tool number.
    Avoiding the rubbish customer service from AluminiumWarehouse since July '13.

  5. #25
    Chaz's Avatar
    Lives in Ickenham, West London, United Kingdom. Last Activity: 7 Hours Ago Has been a member for 4-5 years. Has a total post count of 811. Received thanks 39 times, giving thanks to others 33 times.
    Quote Originally Posted by m_c View Post
    There's not a setting for that. You'll need to ensure however you produce your G-code does the spindle direction setting.

    You could allocate blocks of tool numbers that rotate certain directions, then use the M6 macro to check and set spindle direction depending on tool number.
    Great, I was thinking it might be CAM based. Ill check the settings in Fusion 360. That said, if I run everything 'upside down', I can stick to CW which suits drilling ops. Will also save me from buying a new 16mm boring bar as I can use what I have.

  6. #26
    Chaz's Avatar
    Lives in Ickenham, West London, United Kingdom. Last Activity: 7 Hours Ago Has been a member for 4-5 years. Has a total post count of 811. Received thanks 39 times, giving thanks to others 33 times.
    Struggling with two items.

    Spindle, doesnt like the one plugin. It works oddly if I disable the plugin but then not on restart of Mach. Ive tried the Matty Zee plugin, seems to work, the drive 'stops' if the start up speed is too high (I need to slow down the ramp time perhaps), and the motor speeds / what mach3 thinks its doing dont match. I dont have feedback on the motorspeed at the moment.

    The main other issue is that Fusion CAD is putting some odd code in which is causing me to hit limits. The consensus is to use the Fanuc turning Post Proccesor. It works, no errors, but I get this:-

    I'm less knowledgeable on turning code than milling however what I dont understand is why its moving to X33 in this line - N20 G0 X33. Z1.414. The way my lathe works is X is a negative number at the top and it should be moving to zero. So X-32 will be my current location when homed up top. This is a slant bed lathe, would this be correct? Ive tried to reverse the X direction in the setup on Fusion but gives me the same output.

    %
    O1001
    N10 G98 G18
    N11 G21
    N12 G50 S6000
    N13 G28 U0.


    (FACE1)
    N14 T1313
    N15 G54
    N16 M8
    N17 G98
    N18 G50 S3000
    N19 G96 S200 M3
    N20 G0 X33. Z1.414
    N21 G1 X15.828 F1000.
    N22 X13. Z0.
    N23 X-1.6
    N24 X1.228 Z1.414
    N25 G0 X33.


    (PROFILE1)
    N26 M9
    N27 G98
    N28 G50 S3000
    N29 G96 S200 M3
    N30 G0 X33. Z1.345
    N31 X14.968
    N32 G1 X14.828 F1000.
    N33 X12. Z-0.069
    N34 Z-6.55
    N35 X12.98
    N36 X15.808 Z-5.136
    N37 G0 Z1.404
    N38 X13.828
    N39 G1 X11. Z-0.01 F1000.
    N40 Z-6.55
    N41 X12.
    N42 X14.828 Z-5.136
    N43 G0 Z1.404
    N44 X12.828
    N45 G1 X10. Z-0.01 F1000.
    N46 Z-4.775
    N47 G18 G3 X11. Z-5.798 R1.3
    N48 G1 Z-5.8
    N49 X13.828 Z-4.386
    N50 G0 Z1.404
    N51 X11.828
    N52 G1 X9. Z-0.01 F1000.
    N53 Z-4.535
    N54 G3 X10.5 Z-5.034 R1.3
    N55 G1 X13.328 Z-3.619
    N56 G0 Z1.404
    N57 X10.828
    N58 G1 X8. Z-0.01 F1000.
    N59 Z-4.5
    N60 X8.4
    N61 G3 X9.5 Z-4.622 R1.3
    N62 G1 X12.328 Z-3.208
    N63 G0 Z1.404
    N64 X9.828
    N65 G1 X7. Z-0.01 F1000.
    N66 Z-4.5
    N67 X8.4
    N68 X8.45
    N69 X8.5 Z-4.501
    N70 X11.328 Z-3.087
    N71 G0 Z1.404
    N72 X9.279
    N73 G1 X6.45 Z-0.01 F1000.
    N74 Z-4.5
    N75 X7.5
    N76 X10.328 Z-3.086
    N77 G0 Z1.404
    N78 X8.729
    N79 G1 X5.901 Z-0.01 F1000.
    N80 Z-4.5
    N81 X6.95
    N82 X9.779 Z-3.086
    N83 G0 Z0.614
    N84 X7.729
    N85 G1 X4.901 Z-0.8 F1000.
    N86 Z-5.
    N87 X8.4
    N88 G3 X10. Z-5.8 R0.8
    N89 G1 Z-6.55
    N90 X12.828 Z-5.136
    N91 X13.838
    N92 G0 X33.


    N93 G28 U0. W0.
    N94 M30
    %

    Thanks in advance.

  7. #27
    Chaz's Avatar
    Lives in Ickenham, West London, United Kingdom. Last Activity: 7 Hours Ago Has been a member for 4-5 years. Has a total post count of 811. Received thanks 39 times, giving thanks to others 33 times.
    This is a G0 command, so its machine coordinates? I dont see anything in post processor to tell it not to use these. Not sure actually.

  8. #28
    Chaz's Avatar
    Lives in Ickenham, West London, United Kingdom. Last Activity: 7 Hours Ago Has been a member for 4-5 years. Has a total post count of 811. Received thanks 39 times, giving thanks to others 33 times.
    Ok, based on this, my X is upside down?


    The turret sits on the top. So it should be showing +36, not -36 (relative to the zero line)?

  9. #29
    Chaz's Avatar
    Lives in Ickenham, West London, United Kingdom. Last Activity: 7 Hours Ago Has been a member for 4-5 years. Has a total post count of 811. Received thanks 39 times, giving thanks to others 33 times.
    Ok. Some progress. Firstly, if something has 'professionally' been converted. Check everything.

    X was upside down.
    Steps were wrong. Explains why some circles too big and some too small.

    Still having a lesser issue. I should end up with a 10mm profile but the G Code is not making that happen. The left over sizes are too large. I suspect its something on the Fusion tooling side, its as if its adding in some additional size somewhere. There is nowhere below where I can get a 10mm and 5mm profile. The closes to zero the X goes is X7.729.

    N25 G98
    N26 G97 S4000 M3
    N27 G0 X17. Z1.347
    N28 X12.971
    N29 G1 X12.828 F250.
    N30 X10. Z-0.067
    N31 Z-4.185
    N32 G18 G3 X10.981 Z-4.541 R1.794
    N33 G1 X13.809 Z-3.127
    N34 G0 Z1.404
    N35 X11.828
    N36 G1 X9. Z-0.01 F250.
    N37 Z-4.024
    N38 G3 X10.5 Z-4.335 R1.794
    N39 G1 X13.328 Z-2.921
    N40 G0 Z1.404
    N41 X10.828
    N42 G1 X8. Z-0.01 F250.
    N43 Z-4.
    N44 X8.413
    N45 G3 X9.5 Z-4.084 R1.794
    N46 G1 X12.328 Z-2.67
    N47 G0 Z1.404
    N48 X10.279
    N49 G1 X7.45 Z-0.01 F250.
    N50 Z-4.
    N51 X8.413
    N52 X8.456
    N53 X8.5 Z-4.001
    N54 X11.328 Z-2.586
    N55 G0 Z1.404
    N56 X9.729
    N57 G1 X6.901 Z-0.01 F250.
    N58 Z-4.
    N59 X7.95
    N60 X10.779 Z-2.586
    N61 G0 Z0.62
    N62 X7.729
    N63 G1 X4.901 Z-0.794 F250.
    N64 Z-5.
    N65 X8.413
    N66 G3 X10. Z-5.794 R0.794
    N67 G1 Z-8.544
    N68 X12.828 Z-7.13
    N69 X14.
    N70 G0 X17.

  10. #30
    Chaz's Avatar
    Lives in Ickenham, West London, United Kingdom. Last Activity: 7 Hours Ago Has been a member for 4-5 years. Has a total post count of 811. Received thanks 39 times, giving thanks to others 33 times.
    OK, sorted I believe. Changed from Radius to Diameter mode. Parts are now basically the right size.

Page 3 of 12 FirstFirst 12345 ... LastLast

Similar Threads

  1. Mach Turn
    By Kai in forum CAD & CAM Software
    Replies: 5
    Last Post: 02-08-2016, 01:40 PM
  2. Denford Star Turn 3
    By MarkBrown in forum Workshop & Equipment
    Replies: 2
    Last Post: 02-12-2014, 09:57 PM
  3. Getting the stepper to turn
    By thorphar in forum General Electronics
    Replies: 0
    Last Post: 16-09-2014, 06:48 PM
  4. 11 hours of trying to get the motors to turn, help please
    By Wotsit in forum Stepper & Servo Motors
    Replies: 19
    Last Post: 05-02-2013, 02:07 AM
  5. LED not turn on
    By Awel in forum Motor Drivers & Controllers
    Replies: 1
    Last Post: 06-12-2011, 05:59 AM

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
  •