Each machine will have at least one tool, whether it is a single pen on a plotter or several beam widths on a laser. The codes required to select the tool, turn each tool on and off and any tangential codes are configured in the tool settings.
Machine Attributes - Tool Settings
Tools can be added by right-clicking on the Tool Settings folder in the explorer window and selecting Add. Once a tool has been configured, you can add a new tool based on this one by right-clicking on the existing tool and selecting Add based on. Adding or changing a tool will display the following tool attributes:
General
Name
Enter a unique name for the tool.
Tool type
The tool types available depend on the type of machine selected on the General page of the Plotter Machine Attributes. Tool assignments are as follows:
Counter machine
- Other Tool
- Router Tool
Laser
- Laser Tool
- Other Tool
Mount Cutter
- Angled Knife
- Ink Jet Pen
- Knife
- One-Way Knife
- Other Tool
- Pen
- Router Tool
- Special 45deg. Knife
- V-Groove Tool
Other
- Angled Knife
- Creasing Tool
- Drill Tool
- Finishing Engraving Tool
- Ink Jet Pen
- Knife
- Laser Tool
- One-Way Knife
- Other Tool
- Pen
- Rough Engraving Tool
- Router Tool
- Rule Setter Placement Tool
- Rule Setter Presser Tool
- Saw
- Sloping Engraving Tool
- Special 45deg. Knife
- V-Groove Tool
Plotter
- Ink Jet Pen
- Pen
Sample maker
- Creasing Tool
- Knife
- Other Tool
- Pen
- Router Tool
- V-Groove Tool
Engraving machine
- Finishing Engraving Tool
- Other Tool
- Rough Engraving Tool
- Sloping Engraving Tool
Pick & Place
- Other Tool
Chemical etch machine
- Other Tool
Rule setter machine
- Rule Setter Placement Tool
- Rule Setter Presser Tool
Width
The tool width is used for feedrate selection, pocketing and drill hole processing. In many circumstances you may leave this value as zero if you wish. The point button toggles between the current drawing units (millimetres or inches) and pointages.
Depth
This option is only available for the MultiCAM driver. The required tool depth should be entered as either %<Gn> to access one of the Custom strings, %<PaletteDepth> to use the palette depth or as a real number in plotter units.
Codes
At on
Enter the code to lower the tool head (or switch on the beam).
At off
Enter the code to raise the tool head (or switch off the beam).
At change
Enter the code to make this tool current.
At deselect
Enter the code to deselect the current tool before another tool is selected. In most cases this can be left blank as the machine automatically deselects the tool when a different tool is selected. See your machine documentation for further information.
Stop feed
If the Use stop feed command option is switched on in the Advanced Driver Settings - Advanced Options section, then the code entered here will be output just before the last entity is output for each tool. For example, a machine that places stripping pins into a board might automatically load the next pin into its cartridge as it places the current pin. The Stop feed command would prevent this automatic loading as the final stripping pin is positioned, because the next pin would need to be a different type.
Power reduction
This option is used with the Sequence Attributes function Short line length. If a short line length greater than 0.00mm is set, an option becomes available on the Plot form - Other page Use power reduction. Selecting this option will output the commands contained within this section.
Normal power
As Power reduction, above. If Power reduction is used, the commands contained within this section will be output to return the machine output to normal power.
Low power tool
From the pulldown list specify an alternative tool to use for lines that are shorter than the length specified in the Palette Sequence, Short line length field.
Tool change MCodes on separate lines
This forces the M-codes for each tool change onto a separate output line, as required by some devices. Deselecting this option will reduce the size of the output file, as there will be no line number or carriage return character output for the M-code.
Tangential
When set this option indicates that the tool must be turned before it can move in a different direction. For example, a pen is not a tangential tool but a knife is, because it has to be facing in the direction the tool is moving. By selecting this option, the Tangential page of the form is made available for modification. Note that some controllers are intelligent enough to deal with the properties of tangential tools themselves, so you are able to leave this option unset. See the specific machine documentation for further information. Some machines require the tool to be turned in the direction it is to move. If the tangential option is selected, the following additional options on the tool attributes page become available:
Maximum angle
Enter the maximum angle that the tool can be turned without raising it.
Tool axis
Enter the code for denoting a move around the tool axis; normally this is C.
Angle units
Enter the increments that the tool head will turn. If, for example, a machine requires the tangential angle to be set in increments of 10 degrees, a 90 degree arc sweep would be output as C9, where C is the tool axis.
Angles between -180 and +180
Check this option for controllers that require tool angles to be between -180° and +180° rather than between 0° and 360°.
Specify arc's included angle
Check this option if the controller needs the included angle (sweep) of arcs to be output as part of the arc command. This will be a positive value for counter-clockwise arcs and negative for clockwise. The value will be prefixed with the Tool axis code.
Output arc's end angle
Check this option if the controller needs the angle at the end of the arc instead of the included angle. The value will be prefixed with the Tool axis code.
Tool angle always absolute
Some controllers require the tool angle to be always output in absolute coordinates regardless of the X,Y coordinate system currently in use.
Tangential codes
Following on
Enter the code to switch on tangential following.
Following off
Enter the code to switch off tangential following.
Delays
Delay string
Enter the code causing the tool to pause after moving but before updating the angle.
NC Simulation
The NC Simulation is a tool used to interpret output generated by a Plotter Machine and display it on the screen. This section is used to configure the visibility of each tool shown in the NC Simulation. Alternatively, if you have chosen to view the Intermediate Drawing, you can use either the visibility option or the Master Tool Setting to Display Machine Tools (Post Processor - Output). In this case the entities will be displayed using the tool settings from this section rather than the palette settings for line pattern and colour.
Pattern
This is the line pattern used when displaying geometry output by each tool using NC Simulation. Available line types are:
- Solid
- Dotted
- Dashed
- Dash Dot
- Dash Dot Dot
In addition, any custom Line Styles (configured in the Master Tool Settings) will be displayed in the list. If one of these custom line styles is selected, a configure button will appear enabling the custom line style to be edited.
Colour
This is the colour each tool usage will be displayed as using the NC Simulation. For example, in the Tool Setting shown below the knife tool has had the colour red assigned to it and the line pattern dashed. Running the NC Simulation on the output will show all lines output with the knife tool in a dashed red line.
Engraving Machines
If the Plotter Machine type has been set to Engraving machine then another group of settings can be configured, as shown below.
Engraving tool settings
Tip (d)
This is the diameter of the tool tip. The actual size of the milling or cutting part of the tool will depend on the Angle (A) and the depth that the tool penetrates the material.
Angle (A)
This is the angle of the sides of the tool. It is used to calculate the actual tool cutting size.
Tool overlap
This is the amount of overlap to apply between successive passes with the tool when milling out an area.
Maximum tool life
If a value is specified here then a Replacement tool (as specified below) will be used once the tool has cut this distance.
Replacement tool
The drop-down list will contain all other tools of the same type as the tool being configured. Select the one to use when this tool has reached its maximum tool life, or leave it blank if you don't have a replacement.
Small tool
Similarly, the drop-down list will contain all other tools of the same type. You can optionally specify a tool with a small diameter and it will be used to mill into small corners of a shape to give a better finish.
Single pass only
Typically all entities are milled as a rectangular shape, with the tool diameter being smaller than the entity's channel width. However, if you have a tool that is the same size as the channel, then you can select this option and the entity will be milled with a single pass of the tool. However, this doesn't affect the number of pecks specified on the Engraving Settings page.
See also: Plotter Substitution Codes