Contents

Overview 1

GCodes Summary Table 2

GCodes In Detail 3

Comments 3

Coordinate System 3

Cutter Compensation 3

Feadrate 3

Leadin 3

Linear Motion 4

Scale 4

Surface Intersection 4

Tabs 5

Torch 5

Torch On/Off 5

Torch Position/Motion 5

Sample G-Code: 6

Using the G-Code Parser in PypeServer 7

Validating and Saving the G-Code 7

Finding Errors 7

The JSON format 8

Overview

The pipe cutting machine can be controlled directly using GCode cuts. These cuts are programmed like traditional machining G-Code programs, though most commands are more descriptive.

GCode cuts are typically used when the motion of a cut is defined in CAD as a shape (instead of parameters), or the cut is not easily defined mathematically. Gcodes sources include:

• Cuts imported from CAD exported data where the data is a set of points.

  • DSTV files, which includes Tekla .nc1 files

  • .DXF, DWG, IGES, STEP (customers can create importers for these. See The JSON Format for more information

• Cuts programmed manually by the operator by entering data into the PypeServer cut editor.

• Cuts created programmatically by you or a 3^rd party. (Typically created in JSON format).

GCodes Summary Table

GCodes In Detail

Default values apply if nothing is set in the GCode.

Comments

• //<comment>

Comments can go on a line along, or can follow a command

Coordinate System

• COORDS_CART (default)

Coordinates input are Cartesian Right-Handed system. You can change the coord system with scale. E.g. change to left-handed, set Scale to 1, 1, -1 (reverse Z).

• COORDS_CYL

Cylindrical coordinates (Y down the pipe, X rotation).

Currently not supported. Contact PypeServer if you need this feature.

Cutter Compensation

• COMP_OFF (default)

• COMP_LEFT

• COMP_RIGHT

• COMP_AUTO - the system will use the direction of the cut as it is input to determine the cut side.

NOTE: PypeServer always keeps the cutting torch on the torch swirl "climb mill" side. So as you change from COMP_LEFT to COMP_RIGHT the system will reverse the cut direction of the cut to keep the swirl on the correct side for optimal cutting.

Feadrate

• F <real number greater than zero>

Leadin

• LEADIN_OFF (default)

• LEADIN_ON

NOTES

• If you have a leadin built into the G-Code, make sure this is set to LEADIN_OFF

• Leadins may not always work correctly with GCode. Visually check the lead-ins (and outs) for each cut.

• Using leadin will set your torch pierce angle to the torch settings, so if you are using a static UV torch setting, make sure to set TUV before beginning your cut.

Linear Motion

These apply to COORDS_CART coordinate system

• G01 <x,y,z>

X provides the distance down the pipe. Y and Z provide a vector from the centerline of the pipe that is intersected to the defined surface intersection of the pipe.

• Y is up, Z is towards the viewer (unless SCALE changes the meanings)

• The YZ point does not need to be at the surface intersection of the pipe, as the vector will be lengthened or shortened to the surface intersection.

• The current U and V torch angle settings are applied at this intersection point.

• G01 <x,y,z,x2,y2,z2>

The two xyz points define a line segment in 3D Cartesian space. This segment is used to intersect the inner and outer surfaces of the pipe. Note that the segment points do not need to be at the ID and/or OD of the pipe, as the segment will be extended in both directions to make the intersection.

• In effect there is no "driving" surface, as both surface intersections are defined by the two points.

• G02 <x,y,z,u,v>

This is the same as G01, except with the torch U and V angles updated.

Scale

• SCALE <x,y,z>

Examples:

• SCALE 1,1,1 //this is the default (nothing changes)

• SCALE 1,1,-1 //reverse Z

• SCALE 0.03937, 0.03937, 0.03937 //data is being input in metric,

Surface Intersection

• SURF_ID

• SURF_OD

The G01 and G02 positions do not always define absolute points of intersection on a pipe. This is because a pipe diameter can (and often does) vary from the "ideal" imported or manually design. Surface Intersection defines the surface on which motion points will stay fixed when torch angles are applied. Here are the uses per different input definitions for COORDS_CART:

• G01 <x,y,z> and G02 <x,y,z,u,v>

The YZ is used to determine a vector out from the centerline of the pipe. This vector is intersected with the specified Surface Intersection. The torch U and V angles (TUV) are then applied from that point.

• G01 <x,y,z,x2,y2,z2>

Surface Intersection is unused. See Linear Motion for this input type.

Tabs

• TABS <integer number>

  • Default is zero

  • If TORCH_OFF is used before the end of the cut, TABS will be turned off (set to zero).

Torch

• T_PLASMA

• T_GAS

• T_MARK

• T_ETCH

NOTEs:

• Your machine must be configured with Mark or Etch to use these settings

Torch On/Off

• TORCH_ON

• TORCH_OFF

NOTES:

• If TORCH_OFF is used before the end of the cut, TABS will be turned off (set to zero). This is because TABS is a specific mode of controlling the torch on and off during the cut.

• If Torch ON/OFF is not set at the beginning of cut motion, the system will turn the torch is to be on at the first step.

• If LEADIN is set to on, then torch on will begin at the beginning of the leadin

• If you are using a GAS torch, the system will pause and wait at the first step for the operator to hit go after the torch is ignited and the hole is pierced.

Torch Position/Motion

• TUV <u,v>

  • The u parameter defines the torch angle that lays the torch down along the length of the pipe.

  • The v parameter defines the torch angle that lays the torch out across the pipe

Sample G-Code:

COORDS_CART

COMP_RIGHT

LEADIN_ON

TABS 0

T_PLASMA

SURF_OD

F 40.00

TUV 0.00, 0.00 //this will stay at this setting the entire cut

G01 -0.751, 0.950, 0.000

G01 -0.785, 0.950, 0.000

G01 -0.603, 0.915, -0.254

G01 -0.513, 0.806, -0.504

G01 -0.378, 0.671, -0.673

G01 -0.277, 0.407, -0.858

G01 -0.069, 0.180, -0.933

TORCH_OFF //tab start

G01 0.173, -0.100, -0.945

G01 0.416, -0.356, -0.881

TORCH_ON //tab stop

G01 0.585, -0.574, -0.757

G01 0.705, -0.787, -0.532

G01 0.809, -0.889, -0.336

G01 0.918, -0.950, -0.026

G01 0.861, -0.908, 0.280

G01 0.747, -0.780, 0.543

G01 0.598, -0.610, 0.728

G01 0.357, -0.349, 0.884

G01 0.128, -0.088, 0.946

G01 -0.080, 0.150, 0.938

G01 -0.317, 0.408, 0.858

G01 -0.440, 0.563, 0.766

G01 -0.643, 0.765, 0.563

G01 -0.691, 0.902, 0.297

G01 -0.751, 0.950, 0.000

Using the G-Code Parser in PypeServer

The G-Code parser will appear in the PypeServer Part editor when you are creating or editing a G-Code cut.

Validating and Saving the G-Code

Validate & Save validates the G-Code (and posts errors if there are any), and (whether the data is good or not) saves the G-Code to the server. If "Auto-Validate/Save is checked, this will be done for you after 2 seconds of idle time when inputting data.

• You can uncheck the Auto-Validate/Save checkbox if you want to make changes without continuous validations. If Auto-Validate is unchecked, then remember to validate and save when leaving the cut or you will lose your changes.

Finding Errors

The GCode Parser will parse the gcode file and provide information on parsing errors. Clicking on the error items will take you to the error in the file.

The JSON format

PypeServer saves GCode in a JavaScript Object Notion (JSON) format. This is an industry standard that is an easier format than .xml for less structured data management. This format is recommended if you wish to create your own GCode cuts programmatically. Contact PypeServer to discuss programming requirements and the C# classes defining the JSON Part, Cut and GCode step objects.