Need help with our new DMG Mori C.N.C. lathe
Close
Login to Your Account
Results 1 to 10 of 10
  1. #1
    Join Date
    Aug 2019
    Country
    UNITED STATES
    State/Province
    Nevada
    Posts
    2
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    0

    Default Need help with our new DMG Mori C.N.C. lathe

    Hi everyone,

    We recently purchased a new DMG MORI C.N.C. Lathe. We haven't yet purchased a C.A.M. system so we are still using G Code programming to get it up and running. We are having a problem within the G71 cycle. The tool nose radius in the offset table is .015. That program will run if you bypass the roughing cycle and will run the finish profile. Joshua Burlson from MORI has to leave so he can't help us out. Could someone please review this program and tell us where we are going wrong? Your help would be greatly appreciated. Thank you.

    William

    The alarm Code is P203, D command figure error.


    %
    O0200(SAMPLE PROGRAM)
    G00G20G40G80G99
    M05
    G28U0
    G0G90G53Z-10.
    N1(ROUGH O.D. .015 TNR)
    G0T0101
    G97M3S1000
    G28U0
    G54
    G0X.85Z.1
    M08
    G50S3000
    G96S200

    G71U.06R.003
    G71P10Q20U.01W.003F.008

    N10G0X-.032
    G1Z0F.001
    G03X.069Z-.029R.035
    G1X.4852Z-1.2224
    G03X.500Z-1.3083R.5
    N20G1Z-1.5


    G1X.850
    G0Z.100
    G28U0
    G0G90G53Z-10.
    M09
    M30
    %

  2. #2
    Join Date
    Oct 2012
    Location
    Orange county, CA
    Posts
    89
    Post Thanks / Like
    Likes (Given)
    4
    Likes (Received)
    18

    Default

    do new DMGs use a fanuc style 2 block G71? try a 1 block format, that would be my first guess to change.

  3. #3
    Join Date
    Sep 2010
    Location
    Victoria Australia
    Posts
    3,654
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    1433

    Default

    Quote Originally Posted by William D Keith View Post
    Hi everyone,

    We recently purchased a new DMG MORI C.N.C. Lathe. We haven't yet purchased a C.A.M. system so we are still using G Code programming to get it up and running. We are having a problem within the G71 cycle. The tool nose radius in the offset table is .015. That program will run if you bypass the roughing cycle and will run the finish profile. Joshua Burlson from MORI has to leave so he can't help us out. Could someone please review this program and tell us where we are going wrong? Your help would be greatly appreciated. Thank you.

    William

    The alarm Code is P203, D command figure error.


    %
    O0200(SAMPLE PROGRAM)
    G00G20G40G80G99
    M05
    G28U0
    G0G90G53Z-10.
    N1(ROUGH O.D. .015 TNR)
    G0T0101
    G97M3S1000
    G28U0
    G54
    G0X.85Z.1
    M08
    G50S3000
    G96S200

    G71U.06R.003
    G71P10Q20U.01W.003F.008

    N10G0X-.032
    G1Z0F.001
    G03X.069Z-.029R.035
    G1X.4852Z-1.2224
    G03X.500Z-1.3083R.5
    N20G1Z-1.5


    G1X.850
    G0Z.100
    G28U0
    G0G90G53Z-10.
    M09
    M30
    %
    Hello William,
    I suspect that there is quite a lot wrong with the geometry of the profile shape. I assume that the 0.035 Radius at the Start of the profile is to be tangent with a line drawn at Z Zero and the line described by G1X.4852Z-1.2224; it's not. I assume that the G1X.4852Z-1.2224 is to be tangent to the 0.035 Radius; it's not. I assume that the 0.5 Radius is to be tangent with the G1X.4852Z-1.2224; it's not.

    None of these geometrical errors would stop the program from running as a Finish Pass. However, the 0.035 Radius at the Start would force the profile into a non-monotonous Z profile and should have raised a corresponding error given that non pocketing G71 cycle is probably set via parameter (set “0” for parameter #8110(depending on control model)). The tool path would run as a finish pass, but may not result in the profile shape you're expecting.

    The 0.015 value specified in the Offset Table doesn't come into the matter, as TNR Comp has not been called. Further, depending on the control model, TNR Comp may be ignored in the G71 cycle, but this doesn't relate to your current issue.

    Error P203 relates to the profile shape described. This alarm is raised in the execution of the G71 or G72 cycle if Z-axis movement is generated in the direction opposite to the programmed direction of movement. This will be the case when G03X.069Z-.029R.035 is executed, as the Radius is Not tangent to a line drawn at Z Zero. The Tool Path starts moving in a Z+ direction, notwithstanding that the Radius End Point is in a Z- direction from the Start Point. Accordingly, fix the errors mentioned above, particularly the errors associated with the 0.035 Radius and the program should run.

    @ coyoinu,
    The control can use either format, dependent on Settings.

    Regards,

    Bill

  4. #4
    Join Date
    Aug 2019
    Country
    UNITED STATES
    State/Province
    Nevada
    Posts
    2
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    0

    Default

    Hi Bill,

    Thank you for the response. You are right. There is no tool nose radius comp enacted. I was going by what the applications engineer told us to do. I don't think he really knew, as he wasn't all that familiar with G code programming. I know everyone uses a CAM system for programming. The dimensions I placed in the body of the G71 cycle were taken from an Autocad 2D profile. I double checked the dimensions in main body and they matched what was on the ACAD drawing. Everything is tangent as it should be. With that being said, with TNR enacted, the X axis start point would be X0. This part looks like a bullet projectile. With the information that I provided, what changes would you suggest we do to the program? I really appreciate your response. Thanks again

    William

  5. #5
    Join Date
    Jan 2014
    Country
    UNITED STATES
    State/Province
    Washington
    Posts
    4,393
    Post Thanks / Like
    Likes (Given)
    803
    Likes (Received)
    2366

    Default

    Quote Originally Posted by William D Keith View Post
    ......I was going by what the applications engineer told us to do. I don't think he really knew, as he wasn't all that familiar with G code programming......
    IMO, anyone calling themselves an application engineer ought to know G code programming inside and out.

    If you post the print of the profile you want to cut and the radius of tool you are using, there are several here that can calc the numbers for your path.

  6. Likes Alloy Mcgraw liked this post
  7. #6
    Join Date
    Mar 2006
    Country
    PHILIPPINES
    Posts
    2,342
    Post Thanks / Like
    Likes (Given)
    464
    Likes (Received)
    682

    Default

    Joshua Burlson from MORI has to leave so he can't help us out.
    As bad as I hate to say it, Get used to hearing this as well as the app engineers not knowing coding. Mori is hands down my favorite machines and definitely one of the best on the market but I don't think you could have possibly bought one at a worse time in their history. My best piece of advice for you is to find out where your nearest Ellison office is, take them all out to lunch and be their best buddy.......

    As far as your problem now, As Vancbiker suggested post your geo and someone on here can spit it out.

    It's nice to see I'm not the only one that uses G53 on a lathe now a days

  8. Likes Cycle1000, cameraman liked this post
  9. #7
    Join Date
    Sep 2010
    Location
    Victoria Australia
    Posts
    3,654
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    1433

    Default

    Quote Originally Posted by William D Keith View Post
    Hi Bill,

    Thank you for the response. You are right. There is no tool nose radius comp enacted. I was going by what the applications engineer told us to do. I don't think he really knew, as he wasn't all that familiar with G code programming. I know everyone uses a CAM system for programming. The dimensions I placed in the body of the G71 cycle were taken from an Autocad 2D profile. I double checked the dimensions in main body and they matched what was on the ACAD drawing. Everything is tangent as it should be. With that being said, with TNR enacted, the X axis start point would be X0. This part looks like a bullet projectile. With the information that I provided, what changes would you suggest we do to the program? I really appreciate your response. Thanks again

    William
    Hello William,
    Based on the numbers you have in your first Post listed code, everything is Not tangent. The 0.035 rad at the start is Not tangent with the line described by the G1X.4852Z-1.2224 Block, nor is it tangent with a hypothetical line perpendicular to the machine centre line drawn at Z Zero. Not being tangent with the hypothetical Z Zero line is the reason for your P203 error.

    A Line tangent with a Circle intersects the Circle at one point only. The following picture shows that the hypothetical Z Zero line intersects the 0.035 Rad in two places, as does the G1X.4852Z-1.2224 line; accordingly no tangent. You will also see from the picture that the Tool Path for the 0.035 Rad heads in a Z+ direction before eventually heading in a Z- direction, which is the Z direction of the command for the circular move. That is the reason for the P203 error.

    dmg1.jpg

    Quote Originally Posted by William D Keith View Post
    With that being said, with TNR enacted, the X axis start point would be X0.
    That would also be incorrect. Because the approach is from Z.1, the TRC Tool Path would be to the Right of a line from X0.0 Z0.1 to X0.0 Z0.0 and result in Tit at the face of the work-piece. If TNC were to be used with an approach via a Z move, then the centre of the TNR would have to be at X0.0. The control only knows what you tell it. It could be that the intention was to have a Tit at the Centre Face of the work-piece. Accordingly, specifying X0.0 would be the way to achieve this.


    Regards,

    Bill
    Last edited by angelw; 08-23-2019 at 09:18 AM.

  10. Likes TeachMePlease, cameraman liked this post
  11. #8
    Join Date
    Nov 2014
    Country
    UNITED STATES
    State/Province
    Colorado
    Posts
    2,705
    Post Thanks / Like
    Likes (Given)
    3217
    Likes (Received)
    711

    Default

    Quote Originally Posted by g-coder05 View Post
    As bad as I hate to say it, Get used to hearing this as well as the app engineers not knowing coding. Mori is hands down my favorite machines and definitely one of the best on the market but I don't think you could have possibly bought one at a worse time in their history. My best piece of advice for you is to find out where your nearest Ellison office is, take them all out to lunch and be their best buddy.......

    As far as your problem now, As Vancbiker suggested post your geo and someone on here can spit it out.

    It's nice to see I'm not the only one that uses G53 on a lathe now a days
    I wonder how many 'Peeps" defer to the conversational mode on the NLX(s) ?



    OD roughing cycle …

    AND



    ^^^ This one is a bit hurried.

    Gotta be honest it's hard for anyone to "Compete" with folks that have been finger camming on a turning center for 25, 35, 45 years plus ---> $5 says half of those (these guys in this thread ^^^^^^) dream in G-code. [Major props / salute.].

    personally if it were me and my lathe hard coding was not 100% rock solid, then I'd be tempted to reconstruct my parts using the conversational interface and over a period of weeks or months (almost by osmosis) try to learn what the machine "Prefers" G-code wise , in terms of style, procedure and format for example the G71 cycle.

    Then start editing the generated G-code based programs (from conversational mode) with making tweaks to the G and M codes piece by piece (if I had to). If you are also using a CAD/CAM package for more complex operations then maybe also compare G-code/ program "style" with what the machine attempts to generate from the conversational mode.

    Just finding out what the machine "Wants" and how it wants it rather than springing "surprise" programs on it (as stupid as that sounds). Again the old and younger salts that have 30 years (or equivalent) + dreaming in G code won't have a problem can susss that all out in matter of hours to minutes.

    It's expensive and nice hardware, best to approach it carefully and in a progressive manner (perhaps/captain obvious).

    Doesn't CELOS have the ability to edit and merge programs from different sources directly on the control ?

    Wondering what the online/on control manuals are like in their descriptions for programming the NLX ? It's G-code list and specification and uses thereof ?


    Does the "Bullet" shaped shell have a profile curve (like a parabola) that is a smidge more challenging to get right in conversational mode ?
    __________________________________________________ __

  12. #9
    Join Date
    Sep 2010
    Location
    Victoria Australia
    Posts
    3,654
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    1433

    Default

    Quote Originally Posted by William D Keith View Post
    Hi Bill,
    With the information that I provided, what changes would you suggest we do to the program? I really appreciate your response. Thanks again

    William
    The information you've provided is sketchy, so the following code is for the shape from an educated guess of what you want. The profile in Blue will work on your machine.

    I'm surprised that you didn't report an error relating to the G90s in your program. In your sample program, you've included the Incremental alternative to the Absolute X command. Accordingly, your control won't use X/Z and G90 for Absolute coordinate specification. You need to omit the instances of G90 (shown in Red) from your program.

    Regards,

    Bill

    %
    O0200(SAMPLE PROGRAM)
    G00 G20 G40 G80 G99
    M05
    G28 U0
    G0 G90 G53 Z-10.
    N1(ROUGH O.D. .015 TNR)
    G0 T0101
    G97 M3 S1000
    G28 U0
    G54
    G0 X.85 Z.1
    M08
    G50 S3000
    G96 S200
    G71 U.06 R.003
    G71 P10 Q20 U.01 W.003 F.008
    N10 G00 X-0.0300
    G01 Z0.0000
    G03 X0.0685 Z-0.0414 I0.0000 K-0.0500
    G01 X0.4847 Z-1.2347
    G03 X0.5000 Z-1.3232 I-0.5073 K-0.0885
    G01 Z-1.5000
    N20 G01 X0.8500

    G0 Z.100
    G28 U0
    G0 G90 G53 Z-10.
    M09
    M30
    %

  13. Likes cameraman liked this post
  14. #10
    Join Date
    Sep 2010
    Location
    Victoria Australia
    Posts
    3,654
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    1433

    Default

    Hello William,

    Following is the Start Area of your original Tool Path (shown in Red), superimposed over the Geometry of my Tool Path (shown in White) and the Tool Path (shown in Green).

    ltest1.jpg

    The issue, is that you Started the Profile description with the Tool Compensated in the program for Tool Nose Radius Compensation, then specified the remainder of the Profile without Compensating for the TNR. Its the resulting initial move in a Z+ direction when the 0.035 Radius Move is executed that causes the P203 alarm.

    Had you used I and K Format to define the Centre Location of the Radius, an error relating to the Radius would have been generated and pointed you in the logical direction to correct the program. Using the R Format for Circular Interpolation simply had the Control shift the Centre Location of the Radius to satisfy the Start and End Point Coordinates specified.



    Regards,

    Bill

  15. Likes cameraman liked this post

Tags for this Thread

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
  •