Sidebar
Table of Contents
Import DXF
Imports program in DXF format. Most software for CAD drawing or vector images have option to save design in DXF format. These types of format usually contain vectors, that can be converted to toolpath.
PlanetCNC TNG software will automatically generate toolpath g-code program based on your imported file.
When using this Import feature, user dialog will be displayed. User has option to configure program parameters to suit his machining needs.
Import dialog
General
Units
You can set units as Metric(mm) or Imperial (in) for your design. You can fine tune your units using Scale option.
Scale
Sets scale of your imported DXF design. This comes handy when you need your toolpath to be re-sized or some other units are used.
E.g.: If you design is drawn in centimeters (cm) then select Units as Metric and set Scale to 10.
Origin
Let say we import file of which we do not know its absolute XY [0,0] coordinates.
Generated toolpath will be positioned accordingly, but not necessarily in a way that would suit us.
Bottom Left
Top Left
Center
Bottom Right
Top Right
Loops
You can set number of loops of generated G-code program. Each generated toolpath pass will be repeated for inserted value of loops.
Example: If you insert Loop:3, pass will be repeated for 3 times.
Interpolation
Interpolate
If your file contains elements such as circles, arcs etc.. you can interpolate these elements into short lines by enabling Interpolate option. Arcs and circles will not be using G02/G03 G-code commands but instead G01 G-code commands.
Smooth
Smoothens the toolpath by adding arc G-code commands G02/G03 for smoother motion between the toolpath straight lines.
Sort
Sorts elements of the file, and optimizes generated toolpath.
In other words, this feature will 'search' and calculate shortest path between the elements of the file.
Reverse
Allows Sort feature to use reverse direction while searching for shortest path. This can additionally optimize the toolpath.
Process
Process
Enables all corresponding features below.
Path
Generated toolpath will use centerline path of SVG object as reference.
Stroke
Generated toolpath will use path stroke outline of object as reference.
Fill
Generated toolpath will use fill outline of object as reference.
Union
Generated toolpath will use union outline of two SVG objects as reference.
Offset
Adds offset to generated toolpath. Value can be positive or negative. Basically you can inflate or shrink the toolpath. Checkbox selects sharp or rounded corners.
Tool Change
Tool Change
Generated program will include tool change commands (Tn M6) if file uses layers.
Each layer number will represent dedicated tool number in generated program.
Offset
G43 Hn G-code will be generated after tool change.
Pause
Pause G-code command 'M0' will be added before the tool change command.
Mode
Your design can be in 2D or 3D.
2D
If 2D mode is selected, Height options will be enabled and you will be able to configure height cutting parameters for generated toolpath.
3D
If 3D mode is enabled, Height options will be disabled since it is assumed that are already defined in file (Safe Height option is still available).
UVW, ZXY, YZK
3D mode enables translation of G-code from conventional XYZ plane to UVW, ZXY or YZK plane.
XYZ→UVW
With this option selected, generated G-code program will translate XYZ coordinates to UVW coordinates. This feature is useful for foam cutters, where second tower uses UV coordinates for its motion.
XYZ→ZXY
With this option selected, generated G-code program will be in ZX plane. XYZ coordinates from file will be translated to ZXY.
XYZ→YZX
With this option selected, generated G-code program will be in YZ plane. XYZ coordinates from file will be translated to YZX.
Height
Safe Height
As mentioned in the beginning, when 2D mode is used, then Height parameters can be set.
Safe height is a safety feature which helps with prevention of machine crashing into obstacles that may interfere with machines toolpath. Obstacles could be screws, fixtures, vises etc..
When machine is finished with cutting first shape, it will ascend to safe height and move to next cutting location of second shape. With this option enabled, generated toolpath will include traverse moves performed at safe height.
Start Height
Start height is usually surface of workpiece material. To this height, machine will descend at traverse rate.
Step Down
Depth of first cutting pass. Each new cutting pass will be deeper for this value. To this height, machine will descend at plunge rate.
Cut Height
Deepest cutting depth that machine will cut at.
Software will automatically calculate number of passes to achieve Cut Height depth at Step Down value per pass.
Tabs
Tabs are used for holding element in place during cut.
Enable
Enables tabs.
Distance
Distance between two tabs.
Size
Size of tabs.
Example of tabs:
Speed
Feed Speed
Sets feed speed for generated toolpath. F-word g-code will be generated. Each feed move will be performed at this speed.
Plunge Speed
Set feed speed of plunge moves for generated toolpath. Each feed move in Z- direction (plunge) will be performed at this speed.
Options
Tangent Knife
Enables C axis movement in direction of toolpath for use with tangential knives. Safe Height moves are generated if required.
Outputs
Generated program will include M3, M5, M7, M8, M9 spindle and coolant G-code commands, depending on options selected.
If file uses layers then outputs will be turned ON at beginning and turned OFF at end of layers toolpath.
Spindle
With this option enabled, generated program will include M3 and M5 spindle G-code.
If layers are used in file, toolpath will include M3 G-code at start of layer and M5 G-code at the end of layer.
If no layers are used, spindle G-code will be generated only at the beginning of program and at the end.
Flood
With this option enabled, generated program will include M7 and M9 flood G-code.
If layers are used, toolpath will include M7 g-code at the start of layer and M9 G-code at the end of layer.
If no layers are used, flood G-code will be generated only at the beginning of program and at the end of program.
Mist
With this option enabled, generated program will include M8 and M9 mist g-codes.
If layers are used, toolpath will include M8 G-code at the start of layer and M9 G-code at the end of layer.
If no layers are used, mist G-code will be generated only at the beginning of program and at the end of program.
Speed
With this option enabled, generated program will include S spindle speed G-code.
Bottom - Off
Inserts OFF G-code for Spindle, Flood, Mist, Delay and Pause at the end of cut before moving up to Safe Height.
Spindle
Inserts OFF G-code for spindle M5.
Flood
Inserts OFF G-code for flood M9.
Mist
Inserts OFF G-code for mist M9.
Delay
Inserts Delay G04 P G-code.
Pause
Inserts Pause M00 G-code.
Top - Off
Inserts OFF G-code for Spindle, Flood, Mist (M5, M9), Delay and Pause at the end of cut after moving up to Safe Height.
Spindle
Inserts OFF G-code for spindle M5.
Flood
Inserts OFF G-code for flood M9.
Mist
Inserts OFF G-code for mist M9.
Delay
Inserts Delay G04 P G-code.
Pause
Inserts Pause M00 G-code.
Top - On
Inserts ON G-code for Spindle, Flood, Mist (M3, M7, M8), Delay and Pause before cut, before moving down from Safe Height to cut (or pass) height.
Spindle
Inserts OFF G-code for spindle M5.
Flood
Inserts OFF G-code for flood M9.
Mist
Inserts OFF G-code for mist M9.
Delay
Inserts Delay G04 P G-code.
Pause
Inserts Pause M00 G-code.
Bottom - On
Inserts ON G-code for Spindle, Flood, Mist (M3, M7, M8), Delay and Pause before cut, after moving down from Safe Height to cut (or pass) height.
Spindle
Inserts OFF G-code for spindle M5.
Flood
Inserts OFF G-code for flood M9.
Mist
Inserts OFF G-code for mist M9.
Delay
Inserts Delay G04 P G-code.
Pause
Inserts Pause M00 G-code.