Postprocessor Basics: What the Presetting File Controls

A postprocessor, called a presetting file in CamDRAW, turns toolpaths into text your control understands. Two machines can follow identical toolpaths and still need different files, and that difference is what the postprocessor holds.

Opening one

Click the gear icon at the very top of the CamDRAW docker, next to the logo, then open the Profile tab.

Each profile block has four buttons. The second, Edit, opens the presetting file of that profile in its own window, with all settings grouped into sections.

Before changing anything, use the third button, Export, to save a copy. Editing a working postprocessor without a backup is how a good configuration gets lost.

The sections

General holds the file extension of the output, a description, the comment character and comment style, whether lines are written without spaces, whether output goes to separate files per tool, and a version number.

Commands holds the actual G-code words: rapid movement, linear movement, clockwise and counterclockwise circular movement, spindle off, and the commands for inch and millimetre output. It also sets the sequence in which the movement command appears in a line, and whether it is repeated on every line or only when it changes.

Coordinates defines the axis names, the number formatting behind each, the order in which they appear in a line, the feed and spindle letters, and line numbering with its start value and increment. Rotation and mapping are set here per axis, along with a factor that can reverse the direction of an axis.

Flat machining and Rotation machining hold the settings specific to each: workpiece shape for flat work, and for rotary work the Z zero convention, whether machining happens outside or inside the cylinder, and whether the diameter input is swapped between axes.

Custom lines is where free text is written into the program: program start, program end, operation start, operation end, tool change, cut start and cut end for laser, plasma and waterjet, and the machine setup file.

Workpiece data input renames the fields shown in the docker, so Width and Height can become something more appropriate for your work.

Default values sets the starting values for new operations: safety height, plunge height, depth, engraving height, cutting height, number of cuts, plunge feed, cutting depth, spindle speed, curve precision and the default tool number.

Rendering sets the axis names used in the 3D view and the direction factor for the rotary axis.

Workpiece zero points holds the text written for each of the nine zero point calls, typically G54 for the first, and which one is selected by default.

Coordinates in detail

This section decides what a line of your program actually looks like. Six things are set per axis, plus the feed, spindle and line number columns.

• Name — the letter used for the axis. X, Y and Z normally, A or B for a rotary axis. The Z entry is the height axis of your machine.

• Formatting — how many decimal places the value carries. 0.0000 gives four, 0.000 gives three. Feed is usually 0.00 and spindle a whole number.

• Sequence — the order the columns appear in a line. Changing the numbers reorders the output.

• Rotation — converts a length along that axis into an angle, using the workpiece radius.

• Mapping — treats the axis as rotary but leaves the value as a length, for controls that expect Y to A mapping themselves.

• Factor — multiplies the value. Set it to -1 to reverse the direction of an axis.

• Repeat — writes the coordinate on every line, or only when it changes.

• Output — switches an axis off entirely, for a machine that has no Z or no rotary.

A three decimal setting with repeat switched off produces compact output:

N00010 G01 X12.500 Y30.000 F800

N00011 X14.250

N00012 Y31.750

The same toolpath with repeat switched on writes every axis on every line, which some older controls require:

N00010 G01 X12.500 Y30.000 Z-1.000 F800

N00011 G01 X14.250 Y30.000 Z-1.000 F800

Line numbering is set alongside: a start value and an increment. Setting the increment to 10 produces N00010, N00020 and so on, which leaves room to insert lines by hand.

Commands in detail

The G-code words themselves. Defaults suit most controls, but they are all editable.

• Rapid movement — normally G0

• Linear movement — normally G1

• Clockwise and counterclockwise circular movement — normally G2 and G3

• Turn off spindle — normally M5, written during a tool change and at the end of an operation

• Inch and millimetre output — normally G20 and G21, written according to the CorelDRAW document unit

• Sequence — where the movement command sits within the line

• Repeat — whether the movement command is written on every line or only when it changes

Custom lines in detail

Free text written into the program at defined moments. This is where most machine-specific adaptation happens, and every placeholder is available here.

Program start

Written once at the top. Safety and setup belong here.

(Project: <project>)

(Tools: <tools>)

<units>

G90 G54

G17

M5

G90 sets absolute positioning, G54 the workpiece zero point, G17 the working plane. Whether your control needs all three depends on what it assumes at power-on.

End of program

M5

G0 Z<first_safe_height>

G0 X0 Y0

M30

Spindle off, retract to a safe height, return to the origin, end the program. Some shops park the head away from the work instead, using the toolpath extents placeholders to move clear of whatever was machined.

Tool change

M5

M6 T<t>

(<tool_name>)

M3 S<s>

G43 H<t> Z<first_safe_height>

Stop the spindle, change the tool, restart at the operation's speed, apply tool length compensation. A checkbox in this section skips the block on the first tool operation, which avoids an unnecessary tool change at the start of a job.

Operation start and end

Written around each machining operation. Coolant is the usual case:

(Op <number>: <name>)

M8

and at the end:

M9

Start and end of cut

Only used by contour cutting for laser, plasma and waterjet, written at the beginning and end of every contour. This is what switches the beam on and off.

(Material: <material>)

M3

G4 P<pierce_time>

and at the end of the contour:

M5

The pierce delay gives the beam time to penetrate before movement starts. Without it the cut begins while the material is still being pierced.

Machine setup

Written to a separate file alongside every program, intended to be run before the job. Surface probing, workpiece zero setting and macro calls belong here, and all placeholders are available.

#100 = <nx>

#101 = <ny>

#102 = <gridsize_x>

#103 = <gridsize_y>

M98 P8000

Default values in detail

These are the numbers new operations open with. Filling them in properly is the difference between typing the same figures a hundred times and typing them once.

Safety height, plunge height, start height, depth, engraving height, cutting height, number of cuts, plunge feed rate, cutting depth, spindle speed, curve precision, allowance and the default tool number can all be preset. Leave a field empty and CamDRAW determines a suitable value itself.

Two more settings live here: whether the safety height and the cutting height are approached during contour cutting. Machines with automatic torch height control usually want both switched off.

Also set here is the position of the first measuring point for the probing grid, given as LL, UL, UR or LR for the four corners. For flat machining this is usually LL, bottom left.

Workpiece zero points

Nine slots, each holding the text written for that zero point call. The first is normally G54, the rest G55 through G59 and beyond depending on the control.

A preselection setting decides which is called by default when the profile is chosen. Setting it to 0 means no call is written at all, which is what you want when the machine setup already selects a coordinate system before the program runs.

Workpiece data input

Renames the fields shown in the Workpiece section of the docker. Width and Height are the defaults for flat work, but a preset can call them Width and Length, or anything else that suits the material.

For rotary presets the same applies to Length, Circumference and the diameter field.

Adjusting rather than starting over

Import a preset close to your machine and adjust it, rather than building one from nothing. More than sixty are supplied, and one written for a similar controller is usually a short step from what you need.

To import: on the Profile tab, click the first button on a profile. The directory of supplied presets opens automatically. The file is copied into your settings folder, so the original stays intact.

Testing a change

Generate a small program after every change and open it with the text editor icon in the NC program section. Reading the actual output is faster than reasoning about what a setting should do.

Keep a simple test drawing for this. A rectangle and a circle produce enough movement to show whether the program start, coordinates, feed rates and program end all look right.

When to ask

Adapting a postprocessor to an unusual control is the kind of task where an hour of guessing can be replaced by a short conversation. Our support team helps with this as part of a subscription or licence, and can make adjustments directly.