Results 1 to 7 of 7

Thread: Relative position zero at start up

  1. #1
    Join Date
    Jul 2009
    Posts
    94
    Thanks
    0
    Thanked 8 Times in 8 Posts

    Default Relative position zero at start up

    Fanuc 0i TC on Goodway turning center.

    My customer wants the relative position to be zero when he switches the machine on.

    I set parameter 3104 bit 4(ppd) to a 0. , but the relative position is the same as machine position each time we switch the machine on.

    The reason the customer needs this is because he still programs his machine using G50 to set his tooling offsets,using geometry offsets will be better , but this is the way he wants to remain programming.

    Regards
    Deon

  2. #2
    Join Date
    Jan 2012
    Posts
    346
    Thanks
    0
    Thanked 70 Times in 62 Posts

    Default Re: Relative position zero at start up

    Quote Originally Posted by DEONSKOK View Post
    Fanuc 0i TC on Goodway turning center.

    My customer wants the relative position to be zero when he switches the machine on.

    I set parameter 3104 bit 4(ppd) to a 0. , but the relative position is the same as machine position each time we switch the machine on.

    The reason the customer needs this is because he still programs his machine using G50 to set his tooling offsets,using geometry offsets will be better , but this is the way he wants to remain programming.

    Regards
    Deon
    Hi Deon,

    PPD is actually bite 3, and setting this bit to 1 has the Relative Display preset to that of the Absolute Position Display if:
    1. A manual reference return is performed.
    or
    2. Setting of a coordinate system by G50 (for a T Series G code system A)

    The Relative Position display will not be relevant when the machine is turned on until a Reference Return is done. If the customer wanted to continue to use G50 to set the Work Coordinate System, it would be better for the Relative Display to track the Machine Coordinate System.

    I understand that the customer is always right, but I'm bewildered by those who wish to remain stuck in the past.

    I've had a few clients like this, and I get around them by stating that I'm not exercising my brief correctly unless I demonstrate and explain the many advantages, both from an efficiency, and safety aspect, of using Geometry and Work Shift offsets. The two points that gets them over the edge are:
    1. The fact that programs can be created without any reference to Tool Position, as one must do when using G50 to set the Work Coordinate System.
    and
    2. The control knows exactly were the tool is, just by calling the tool with its offset, irrespective of where the Tool Change Position is.

    Regards,

    Bill

  3. #3
    Join Date
    Jul 2009
    Posts
    94
    Thanks
    0
    Thanked 8 Times in 8 Posts

    Default Re: Relative position zero at start up

    Thank you for your reply Bill.

    You mention customers , do you do cnc training for a machine tool company.


    Regards
    Deon

  4. #4
    Join Date
    Jan 2012
    Posts
    346
    Thanks
    0
    Thanked 70 Times in 62 Posts

    Default Re: Relative position zero at start up

    Quote Originally Posted by DEONSKOK View Post
    Thank you for your reply Bill.

    You mention customers , do you do cnc training for a machine tool company.


    Regards
    Deon
    Hi Deon,
    I write Software, I have my own Editor/Comms, CAM and Program Verification software. I also write custom software for automation applications. I provide training and methodology for anyone that stands still for long enough to listen to me. Many of the machine tool companies use my services.

    Regards,

    Bill

  5. #5
    Join Date
    Jul 2009
    Posts
    94
    Thanks
    0
    Thanked 8 Times in 8 Posts

    Default Re: Relative position zero at start up

    Hello Bill

    Please give us the name of your verification software , and can it be viewed on line.

    I believe there is a need for backplotting software , so that a person can check a program graphically before scrapping a job or damaging a machine.

    Returning to my original request.

    I have a Goodway (Yama Seiki) machine with a 0i TD control , parameter 3104 bit 3 (ppd) set to 0.

    I move the z axis to a position.
    Press pos.
    press Rel.
    Press w.
    Press origin.
    W is now 0.
    Switch off machine.
    Switch on machine.
    W still zero before I reference machine.



    Next to this machine is an older model with a 0i TC control.

    parameter 3104 bit 3 (ppd) set to 0.


    I move the z axis to a position.
    Press pos.
    press Rel.
    Press w.
    Press origin.
    W is now 0.
    Switch off machine.
    Switch on machine.
    W is the same value as machine position ,before referencing.

    The customer needs the w position to be zero when swithing on.

    Any advice

    Regards
    Deon

  6. #6
    Join Date
    Jan 2012
    Posts
    346
    Thanks
    0
    Thanked 70 Times in 62 Posts

    Default Re: Relative position zero at start up

    Hi Deon,
    The software is a Suite comprising CAM, Program Verification and Editor/Comms; I'm won't be splitting them up in the short term.

    Over the last year, I've embarked on a major rewrite to accommodate 64 bit Operating Systems. Accordingly, the software is in test at a number of engineering shop. I'll send you a copy in the next few months if you care to PM me your email address.

    With regards to the Relative Position Display, I believe you will find the difference between the two machine is the type of encoder used by each, with the newer machine using an Absolute Encoder. I haven't had time to check, but I can't recall a parameter that will alter the way the older machine behaves.

    With regards to establishing a coordinate system using G50, its important that the G50 block be executed at a known same position for each tool used in the program; as I'm sure you know. The most convenient position to do this from is the Zero Return Position (G28), or any of the additional Reference Return positions accessible via G30. This is because its a rock solid repeatable position that can be reclaimed easily should the program be aborted for any reason.

    Not all machines will have the Subsequent Reference Return function via G30 (its an option), and if this is the case, using the G28 Reference Return may not be an efficient tool change position if short work is being carried out on a relatively long machine. Many get around this by establishing a tool change position an incremental distance away from the Reference Position as follows:

    /G28 U0.0 W0.0
    /G00 U-100.0 X-300.0
    G50 T0100 S3500
    G50 X_ Z_
    G96 S250 M03
    G00 X150.0 Z10.0 T0101 M08
    ----------
    ----------
    ----------
    ----------
    G00 X_ Z_ T0100 M09
    M01
    etc

    The blocks in block delete are only executed at the initial start of the program and if the program is aborted and Reset for some reason. I have another method that is far more fool proof involving long and short G50 locations, but its a bit long winded to explain it here.

    I still can't quite see what the importance is that the Relative Position display be Zero once set and the power off/on cycled.

    Most machine's Machine Coordinate Display will be X0.0 Z0.0 when the slides are at the Reference Return Position. That being the case, the coordinate to establish the G50 is easily got by using the Machine Position Coordinates, or the Relative Coordinates set to Zero at the Reference Return Position. For example, if the G50 for an OD turning tool is being gained, the following is one of many methods:

    1. With workpiece mounted in chuck, start the spindle and cut a diameter long enough to measure conveniently.

    2. Clear the tool of the workpiece in the Z axis only, stop the spindle and measure the freshly cut diameter.

    3. Because the Machine Position Display is Zero when the slides are at Reference Return, the display will now be showing the current distance the tool is from the Reference position, via a negative number.

    4. Add to the current X Machine Coordinate the measured diameter as a negative value. The result will be the X G50 in negative form. The positive form of this number will be used as the G50 X in the program if the Tool Change is executed at the X Reference Return Position.

    5. Start the Spindle and take a light cut on the face of the Workpiece. Clear the tool of the work in X only, stop the spindle and measure the amount of material between the Current Z location of the tool and Z Zero of the work. This amount is added as a negative value to the current negative Z Machine Coordinate. The resulting number will be the Z G50 in negative form. The positive form of this number will be used as the G50 Z in the program if the Tool Change is executed at the Z Reference Return Position.

    6. Repeat from 1 to 5 for all other tools to be set.

    7. If the Tool Change position is to be a Relative distance away from the Reference Return location, simply subtract the required X Z distance from the G50 Coordinates gained above.

    8. Its rare that the G50 Coordinates are whole numbers. If the machine is being used in Metric Configuration, I use the Integer component of the Real Number as the G50 in the program, and the decimal component as an offset. This results in a clean number in the program and a small offset (max 0.999mm - less than 0.040"). If the machine is used in Imperial Mode, I round to the closest 0.5" and use that number in the G50 and the difference as an offset.

    9. Convince the client to come in out of the cold and become familiar with Geometry Offset Programming.

    Regards,

    Bill
    Last edited by angelw; 03-15-12 at 04:28 PM.

  7. #7
    Join Date
    Jul 2009
    Posts
    94
    Thanks
    0
    Thanked 8 Times in 8 Posts

    Default Re: Relative position zero at start up

    Hello Bill

    Thank you.

    Regards
    Deon

Similar Threads

  1. Auto operation cant cycle start alarm occurs when cycle start is pushed.
    By Petro in forum General CNC & Manufacturing Discussion
    Replies: 1
    Last Post: 10-10-12, 10:28 AM
  2. Haas VF-6 Start Up Problem
    By ssred in forum Machine Repair & Troubleshooting
    Replies: 4
    Last Post: 01-08-10, 02:11 PM
  3. Fanuc 10 start-up problem
    By TerryID in forum Fanuc Controls
    Replies: 2
    Last Post: 12-02-09, 12:48 PM
  4. double start thread
    By jmaxa in forum Programming / Applications
    Replies: 4
    Last Post: 07-16-09, 01:11 PM
  5. 6 start thread
    By Moddyboddy in forum Programming / Applications
    Replies: 0
    Last Post: 05-31-08, 09:50 AM

Posting Permissions

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