13 January 2016 Using CamBam with plasma cutters

CamBam works great with plasma cutters. Here are some settings and tips we use to drive our own plasma cutter.

Plasma resource files

Download plasma resource files

The resource file contains a post processor definition, a CAM style library and a drawing template.
These files need to be copied into subfolders of the CamBam system folder. This is typically located at:

C:\ProgramData\CamBam plus 0.9.8
To find this location, use the Tools - Browse system folder menu command from within CamBam.

Unzip the resource files, then copy...
Plasma.cbpp to (system folder)\post
Plasma-mm.xml to (system folder)\styles
plasma.cb to (system folder)\templates

Restart CamBam and you are now ready to start working with plasma.

Working with plasma

To start a plasma drawing, use the File - New From Template menu command, then select the plasma.cb file.

This drawing is set to refer to the plasma CAM style library and post processor.

A 100mm square is included, which is linked to a profile machining operation. The square can be replaced with your own shapes, then relinked to the machining operation by selecting and dragging the drawing objects in the drawing tree, onto the profile machining operation.

Save the drawing and generate g-code. We are now all set for cutting!

Plasma hardware does vary, so you should check and customise the plasma post processor to make sure any g-code produced is suitable for your machine.

Insides and Outsides

Profile machining operations will automatically detect inside and outside shapes. For example, if you select two shapes; a circle within a square, then insert a profile operation, CamBam will realise that the circle should be cut first. If the profile is set to an Outside cut, then the inside circle will be cut on the Inside of the line and the outer square will be cut on the Outside of the shape. If the profile is set to Inside the reverse is true.

Multiple shapes can be selected (insides and outers), and a single profile machining operation inserted to cut them.

Machining styles

The profile machining operation inherits all its properties from the default (blank named) style in the Plasma-mm style library. If the default style is customised to suit your most common plasma operations, no further changes may be needed to the machining operations in the drawing.

To create a new machining style, alter the properties of the profile machining operation to suit your operation. For example, reduce the Cut Feedrate when cutting thicker plate.

To make the modified style available to this and other drawings:

  • Right click the machining operation, then select Copy
  • Select the System tab at the top of the drawing tree, then expand the CAM Styles folder.
  • Right click the Plasma-mm style, then select New CAM style.
  • Rename the new style to something meaningful, such as '5mm plate'.
  • Right click the new style and select Paste format. This will copy the properties set in your machining operation into the new style.
The '5mm plate' style will now be available to all your drawings. To make use of it in the current drawing...
  • Switch back to the Drawing tab at the top of the drawing tree.
  • Right click the profile machining operation, then select Reset to defaults.
    This ensures any changes you make to the style will automatically be available to the machining operation.
  • Edit the machining operation's Style property, and from the drop down list select 5mm plate.

Plasma post processor

One main difference between the plasma post and a standard machining post is that the spindle on/off commands have been moved from the header and footer sections into the Start Cut and End Cut properties. In these sections we can add codes to turn the plasma on and off, typically with M3 and M5 g-codes.

The header section also includes a Z touch off (probe) sequence that zeros the Z DRO to the top of the plate. This sequence should only be used if suitable hardware such as a floating Z and Z limit switch are in place.


{$comment} {$cbfile.name} {$date} {$endcomment}
{$units} {$distancemode} {$velocitymode}}
( move to the X,Y location of first toolpath )
G0 X{$mop.first.X} Y{$mop.first.y}
( do a Z probe cycle )
G31 Z-100 F1000
( set this as Z=0 )
G92 Z0
( retract 5mm until tip clears plate )
G0 Z5.0
( set this as Z=0 )
G92 Z0

Important! The 5mm retract height should be adjusted to the target machine. This is the distance the Z needs to move after the limit switch is triggered so that the tip lies just above the plate surface.

The G31 probe plunge feedrate should also be checked. This feedrate should be set to a value where the probe cycle executes reliably, without risk of damaging the cutter tip.

Start Cut

( pierce height )
G0 Z5
( torch on )
( plunge to cutting depth )
G1 Z{$mop.targetdepth} F{$mop.plungefeedrate}

For thicker plate, a pause may be required at the end of the Start Cut, (eg G4 P500), to give the plasma time to pierce the plate. In our setup, we find setting the plunge feedrate to a suitable speed has a similar effect.

End Cut

( torch off )
( small delay - ms )
G4 P500

The small delay in the end cut section is useful in setups (such as ours), where the torch detect voltage takes a little while to die away.

Important! For the start and end cut states to work correctly, the machining operation must specify a target depth that is below its stock surface value. It is the action of the Z move going below stock surface that triggers the start cut event. To prevent having to remember to set these parameters for each machining operation, default stock surface and target depth values are set in the plasma CAM style library.

Plasma CAM style library

The following table describes the setting used for the default style of our Plasma-mm CAM style library.

This is a metric library, so all units are described in millimeters.

Only the default style is shown which should be set with values used for the most common plasma cutting operation (in our example 3mm steel plate). More CAM styles can be added for different operations, then selected in the machining operation's Style property.

Stock Surface = 1.6
Target Depth = 1.5

In order for the Start Cut and End Cut states to be detected, the target depth needs to be below the stock surface value.
The Target Depth property should be set to the 'standoff' cutting height above the plate that is recommended for your equipment.
The actual cutting height is typically controlled and dynamically adjusted using a THC (Torch Height Control) system.

Cut Feedrate = 1400 Generally the faster you are able to cut for a given plate thickness the better. However it can be a trade-off between amount of spatter generated and the taper of a cut.
For smaller holes, a reduced feedrate is advised as this will reduce cut taper.
Plunge Feedrate = 1000 The plunge feedrate is used as the cutter moves from the pierce height to the cutting height.
It should be slow enough so the plasma has time to pierce the plate.
Lead In/Out Move
Lead Move Type = Tangent
Tangent Radius = 2mm
Tangent lead in and out moves are used as these keep the pierce point away from the cutting line.
Milling Direction = Climb Surprisingly, the direction of cut can affect the quality of cut.
For an outside cut, with milling direction set to Climb, the cut will move clockwise around the shape.
For milling direction set to Conventional, the cut will move anti-clockwise around the shape.
Tool Diameter = 1.6 Tool diameter should be set to the plasma cut width (kerf) of a typical cut.
Copyright (c) 2017 HexRay Ltd