Announcements
Attention for Customers without Multi-Factor Authentication or Single Sign-On - OTP Verification rolls out April 2025. Read all about it here.

Doosan Mill/Turn Y axis milling issues

ubi.james13
Enthusiast

Doosan Mill/Turn Y axis milling issues

ubi.james13
Enthusiast
Enthusiast

Hi, would like to mill a part  similar to the attached part using  Y axis rather than using polar co-ordinates  but our machine only has 20mm below  X so I've programmed two processes with X reversed on one, both work great if run on there own but will not run as single programme . I can see the issue, it is because I'm using the same tool there is no tool Clarence and no G369  Compensation Cancel before it turns it back on

Not sure if this is a post problem or user error 

Any help much apricated 

 

https://a360.co/3JeshgB

0 Likes
Reply
Accepted solutions (1)
521 Views
6 Replies
Replies (6)

seth.madore
Community Manager
Community Manager

At these moves here:

G3 Y1.0602 Z0.0224 J0.0598 K0.0199
G1 Y1.12 Z0.0423
G0 X7.1654

(2D CONTOUR2)
M190
G368 X0. Z0. D1. B90. W8
G0 C180.
M189
G1 X7.1654 Y-1.12 Z0.0423 F470.

 

What is missing from where?


Seth Madore
Customer Advocacy Manager - Manufacturing
0 Likes

ubi.james13
Enthusiast
Enthusiast

Hi @seth.madore 

Have had a play with programs so attached is a full working hand edited programme and also the original un-edited. I'm guessing the post needs editing to achieve the same results, can you help? Should add although I have used  Fusion360 for some years I've never before used for Lathe parts only milling having only programmed Mazatrol lathes so this Fanuc Doosan is proving to be a challenge being new to G code lathe programming and a new machine so forgive me if I seem a bit slow !

0 Likes

bob.schultz
Autodesk
Autodesk
Accepted solution

Hello @ubi.james13,

 

I don't know if the tool and spindle blocks have to be reinstated or not.  I am attaching your program with just the G369 added, can you let me know if this runs on your machine?  If so, you can add a single line to the post to get this output.

 

    } else {
      if (getProperty("useG400") && ((bFormat.getResultingValue(abc.y) == 0) || (Math.abs(bFormat.getResultingValue(abc.y)) == 90))) {
        setSpindleOrientationMilling(abc);
      } else {
        cancelWorkPlane();  // <<< ADD THIS LINE
        var compensationOffset = tool.isTurningTool() ? tool.compensationOffset : tool.lengthOffset;
        var toolAxisMode = (machineState.usePolarMode || machineState.useXZCMode || machineState.axialCenterDrilling) ? 0 : 1;  // D0 = tool axis is Z-axis, D1 = tool axis is X-axis
        gWCSModal.reset();
        writeBlock(
          gWCSModal.format(368),
          "X" + spatialFormat.format(0),
          "Z" + spatialFormat.format(0),
          "D" + spatialFormat.format(toolAxisMode),
          bFormat.format((getSpindle(PART) == SPINDLE_MAIN) ? abc.y : -abc.y), // only B-axis is supported for G368
          "W" + compensationOffset
        );
      }

Please let me know if it works and we will update the library post.



Bob Schultz
Sr. Post Processor Developer

1 Like

ubi.james13
Enthusiast
Enthusiast

Hi @bob.schultz ,no my machine definitely needs to reinstate the tool and spindle code, after the G369 the upper turret returns to home in X & Y with a spindle stop. The good news is I have found a work-around on the part I'm actually machining for the moment by doing all the work on one side of the part then going back to do other side ! as long as this requires a tool change all code runs straight from post !  

0 Likes

bob.schultz
Autodesk
Autodesk

Thanks @ubi.james13, this is good to know.  We will get the library post updated.  For your information, you can force a tool change using a Manual NC command prior to an operation, which will allow you to program the operations in the desired order.  This will also output the G369 code.

 

bobschultz_0-1647522646658.png

 



Bob Schultz
Sr. Post Processor Developer

1 Like

ubi.james13
Enthusiast
Enthusiast

@bob.schultz yeah works a treat !

0 Likes