The Path workbench offers tools to import, create, manipulate and export machine toolpaths in FreeCAD. With it, the user is able to import, visualize and modify existing G-code programs, generate toolpaths from 3D shapes, and export these toolpaths to G-code.
The Path workbench is currently in early development, and does not offer all the advanced functions found in some commercial alternatives. However, the Python scripting interface makes it easy to modify or develop more powerful tools.
FreeCAD's Path objects are made of a sequence of motion commands. A typical use is this:
>>> import Path
>>> c1 = Path.Command("g1x1")
>>> c2 = Path.Command("g1y4")
>>> c3 = Path.Command("g1 x2 y2") # spaces end newlines are ignored
>>> p = Path.Path([c1,c2,c3])
>>> o = App.ActiveDocument.addObject("Path::Feature","mypath")
>>> o.Path = p
>>> print (p.toGCode())A preliminary concept is important to grasp. Most of the implementation below relies heavily on motion commands that have the same names as G-code commands, but aren't meant to be close to a particular controller's implementation. Names such as 'G0' to represent 'rapid' move or 'G1' were chosen to represent 'feed' move for performance (efficient file saving) and to minimize the work needed to translate to/from other G-code formats. Since the CNC world speaks thousands of G-code dialects, a very simplified subset of it was chosen. You could describe FreeCAD's G-code format as a "machine-agnostic" form of G-code.
Inside .FCStd files, Path data is saved directly into that G-code form.
All translations to/from dialects to FreeCAD G-code are done through pre- and post- scripts. That means that if you want to work with a machine that uses a specific LinuxCNC, Fanuc, Mitusubishi, or HAAS controller etc, you will have to use (or write if nonexistent) a post processor for that particular controller (see the "Importing and exporting G-code" section below).
The following rules and guidelines define the G-code subset used internally in FreeCAD:
-
G-code data, inside FreeCAD Path objects, is separated into "Commands". A Command is defined by a command name, which must begin with G or M, and (optionally) arguments, which are in the form Letter plus a Float, for example X 0.02 or Y 3.5 or F 300. These are examples of typical G-code commands in FreeCAD:
G0 X2.5 Y0 (The command name is G0, the arguments are X=2.5 and Y=0)
G1 X30 (The command name is G1, the only argument is X=30)
G90 (The command name is G90, there are no arguments)
-
For the numeric part of a G or M command, both "G1" or "G01" forms are supported.
-
Only commands starting with G or M are supported at the moment.
-
Only millimeters are accepted at the moment. G20/G21 are ignored.
-
Arguments are always sorted alphabetically. This means that if you create a command with "G1 X2 Y4 F300", it will be stored as "G1 F300 X2 Y4"
-
Arguments cannot be repeated inside a same command. For example, "G1 X1 Y2 X2 Y3" will not work. You will need to split it into two commands, for example: "G1 X1 Y2, G1 X2 Y3"
-
X, Y, Z, A, B, C arguments are absolute or relative, depending on the current G90/G91 mode. Default (if not specified) is absolute.
-
I, J, K are always relative to the last point. K can be omitted.
-
X, Y, or Z (and A, B, C) can be omitted. In this case, the previous X, Y or Z coordinates are maintained.
-
G-code commands other than the ones listed in the table below are supported, that is, they are saved inside the path data (as long as they comply to the rules above, of course), but they simply won't produce any visible result on screen. For example, you could add a G81 command, it will be stored, but not displayed.
Command Description Supported Arguments Displayed
G0 rapid move X,Y,Z,A,B,C Red
G1 normal move X,Y,Z,A,B,C Green
G2 clockwise arc X,Y,Z,A,B,C,I,J,K Green
G3 counterclockwise arc X,Y,Z,A,B,C,I,J,K Green
G81, G82, G83 drill X,Y,Z,R,Q Red/Green
G38.2 Straight probe move (used in probe operation) Z,F Yellow
G90 absolute coordinates
G91 relative coordinates
(Message) comment
The Command object represents a G-code command. It has three attributes: Name, Parameters and Placement, and two methods: toGCode() and setFromGCode(). Internally, it contains only a name and a dictionary of parameters. The rest (placement and gcode) is computed to/from this data.
>>> import Path
>>> c=Path.Command()
>>> c
Command ( )
>>> c.Name = "G1"
>>> c
Command G1 ( )
>>> c.Parameters= {"X":1,"Y":0}
>>> c
Command G1 ( X:1 Y:0 )
>>> c.Parameters
{'Y': 0.0, 'X': 1.0}
>>> c.Parameters= {"X":1,"Y":0.5}
>>> c
Command G1 ( X:1 Y:0.5 )
>>> c.toGCode()
'G1X1Y0.5'
>>> c2=Path.Command("G2")
>>> c2
Command G2 ( )
>>> c3=Path.Command("G1",{"X":34,"Y":1.2})
>>> c3
Command G1 ( X:34 Y:1.2 )
>>> c3.Placement
Placement [Pos=(34,1.2,0), Yaw-Pitch-Roll=(0,0,0)]
>>> c3.toGCode()
'G1X34Y1.2'
>>> c3.setFromGCode("G1X1Y0")
>>> c3
Command G1 [ X:1 Y:0 ]
>>> c4 = Path.Command("G1X4Y5")
>>> c4
Command G1 [ X:4 Y:5 ]
>>> p1 = App.Placement()
>>> p1.Base = App.Vector(3,2,1)
>>> p1
Placement [Pos=(3,2,1), Yaw-Pitch-Roll=(0,0,0)]
>>> c5=Path.Command("g1",p1)
>>> c5
Command G1 [ X:3 Y:2 Z:1 ]
>>> p2=App.Placement()
>>> p2.Base = App.Vector(5,0,0)
>>> c5
Command G1 [ X:3 Y:2 Z:1 ]
>>> c5.Placement=p2
>>> c5
Command G1 [ X:5 ]
>>> c5.x
5.0
>>> c5.x=10
>>> c5
Command G1 [ X:10 ]
>>> c5.y=2
>>> c5
Command G1 [ X:10 Y:2 ]The Path object holds a list of commands
>>> import Path
>>> c1=Path.Command("g1",{"x":1,"y":0})
>>> c2=Path.Command("g1",{"x":0,"y":2})
>>> p=Path.Path([c1,c2])
>>> p
Path [ size:2 length:3 ]
>>> p.Commands
[Command G1 [ X:1 Y:0 ], Command G1 [ X:0 Y:2 ]]
>>> p.Length
3.0
>>> p.addCommands(c1)
Path [ size:3 length:4 ]
>>> p.toGCode()
'G1X1G1Y2G1X1'
lines = """
G0X-0.5905Y-0.3937S3000M03
G0Z0.125
G1Z-0.004F3
G1X0.9842Y-0.3937F14.17
G1X0.9842Y0.433
G1X-0.5905Y0.433
G1X-0.5905Y-0.3937
G0Z0.5
"""
slines = lines.split('\n')
p = Path.Path()
for line in slines:
p.addCommands(Path.Command(line))
o = App.ActiveDocument.addObject("Path::Feature","mypath")
o.Path = p
# but you can also create a path directly form a piece of G-code.
# The commands will be created automatically:
p = Path.Path()
p.setFromGCode(lines)As a shortcut, a Path object can also be created directly from a full G-code sequence. It will be divided into a sequence of commands automatically.
>>> p = Path.Path("G0 X2 Y2 G1 X0 Y2")
>>> p
Path [ size:2 length:2 ]The Path feature is a FreeCAD document object, that holds a path, and represents it in the 3D view.
>>> pf = App.ActiveDocument.addObject("Path::Feature","mypath")
>>> pf
<Document object>
>>> pf.Path = p
>>> pf.Path
Path [ size:2 length:2 ]The Path feature also holds a Placement property. Changing the value of that placement will change the position of the Feature in the 3D view, although the Path information itself won't be modified. The transformation is purely visual. This allows you, for example, to create a Path around a face that has a particular orientation on your model, that is not the same orientation as your cutting material will have on the CNC machine.
However, Path Compounds can make use of the Placement of their children (see below).
NOTE: This type of tool usage is depreciated as of the 0.19 official release. In 0.19 the new ToolBit tool system was implemented to supersede this older, Legacy, system. Therefore, coding has changed from what is represented below. Please visit Path Tools page for more information.
===Scripting <= 0.18===
The Tool object contains the definitions of a CNC tool. The Tooltable object contains an ordered list of tools. Tooltables are attached as a property to Path Project features, and can also be edited via the GUI, by double-clicking a project in the tree view, and clicking the "Edit tooltable" button in the task views that opens.
From that dialog, tooltables can be imported from FreeCAD's .xml and HeeksCad's .tooltable formats, and exported to FreeCAD's .xml format.
>>> import Path
>>> t1=Path.Tool()
>>> t1
Tool Default tool
>>> t1.Name = "12.7mm Drill Bit"
>>> t1
Tool 12.7mm Drill Bit
>>> t1.ToolType
'Undefined'
>>> t1.ToolType = "Drill"
>>> t1.Diameter= 12.7
>>> t1.LengthOffset = 127
>>> t1.CuttingEdgeAngle = 59
>>> t1.CuttingEdgeHeight = 50.8
>>> t2 = Path.Tool("my other tool",tooltype="EndMill",diameter=10)
>>> t2
Tool my other tool
>>> t2.Diameter
10.0
>>> table = Path.Tooltable()
>>> table
Tooltable containing 0 tools
>>> table.addTools(t1)
Tooltable containing 1 tools
>>> table.addTools(t2)
Tooltable containing 2 tools
>>> table.Tools
{1: Tool 12.7mm Drill Bit, 2: Tool my other tool}
>>> The aim of this feature is to gather one or more toolpaths and associate it (them) with a tooltable. The Compound feature also behaves like a standard FreeCAD group, so you can add or remove objects to/from it directly from the tree view. You can also reorder items by double-clicking the Compound object in the Tree view, and reorder its elements in the Task view that opens.
>>> import Path
>>> p1 = Path.Path("G1X1")
>>> o1 = App.ActiveDocument.addObject("Path::Feature","path1")
>>> o1.Path=p1
>>> p2 = Path.Path("G1Y1")
>>> o2 = App.ActiveDocument.addObject("Path::Feature","path2")
>>> o2.Path=p2
>>> o3 = App.ActiveDocument.addObject("Path::FeatureCompound","compound")
>>> o3.Group=[o1,o2]An important feature of Path Compounds is the possibility to take into account the Placement of their child paths or not, by setting their UsePlacements property to True or False. If not, the Path data of their children will simply be added sequentially. If True, each command of the child paths, if containing position information (G0, G1, etc..) will first be transformed by the Placement before being added.
Creating a compound with just one child path allows you therefore to turn the child path's Placement "real" (it affects the Path data).
The Path project is an extended kind of Compound, that has a couple of additional machine-related properties such as a tooltable. It is made mainly to be the main object type you'll want to export to G-code once your whole path setup is ready. The Project object is now coded in Python, so its creation mechanism is a bit different:
>>> from PathScripts import PathProject
>>> o4 = App.ActiveDocument.addObject("Path::FeatureCompoundPython","prj")
>>> PathProject.ObjectPathProject(o4)
>>> o4.Group = [o3]
>>> o4.Tooltable
Tooltable containing 0 toolsThe Path module also features a GUI tooltable editor that can be called from Python, giving it an object that has a ToolTable property:
>>> from PathScripts import TooltableEditor
>>> TooltableEditor.edit(o4)Assign the shape of wire Part to a normal Path object, using Path.fronShape() script function (or more powerful Path.fronShapes()). By giving as parameter a wire Part object, its path will be automatically calculated from the shape. Note that in this case the placement is automatically set to the first point of the wire, and the object is therefore not movable anymore by changing its placement. To move it, the underlying shape itself must be moved.
>>> import Part
>>> import Path
>>> v1 = FreeCAD.Vector(0,0,0)
>>> v2 = FreeCAD.Vector(0,2,0)
>>> v3 = FreeCAD.Vector(2,2,0)
>>> v4 = FreeCAD.Vector(3,3,0)
>>> wire = Part.makePolygon([v1,v2,v3,v4])
>>> o = FreeCAD.ActiveDocument.addObject("Path::Feature","myPath2")
>>> o.Path = Path.fromShape(wire)
>>> FreeCAD.ActiveDocument.recompute()
>>> p = o.Path
>>> print(p.toGCode())Both Path::Feature and Path::FeatureShape features have a Python version, respectively named Path::FeaturePython and Path::FeatureShapePython, that can be used in Python code to create more advanced parametric objects derived from them.
G-code files can be directly imported and exported via the GUI, by using the "open", "insert" or "export" menu items. After the file name is acquired, a dialog pops up to ask which processing script must be used. It can also be done from Python:
Path information is stored into Path objects using a subset of G-code described in the "FreeCAD's internal G-code format"section above. This subset can be imported or exported "as is", or converted to/from a particular version of G-code suited for your machine.
If you have a very simple and standard G-code program, that complies to the rules described in the "FreeCAD's internal G-code format" section above, for example the boomerang from cnccookbook, it can be imported directly into a Path object, without translation (this is equivalent to using the "None" option of the GUI dialog):
import Path
f = open("/path/to/boomerangv4.ncc")
s = f.read()
p = Path.Path(s)
o = App.ActiveDocument.addObject("Path::Feature","boomerang")
o.Path = pIn the same manner, you can obtain the path information as "agnostic" G-code, and store it manually in a file:
text = o.Path.toGCode()
print text
myfile = open("/path/to/newfile.ngc")
myfile.write(text)
myfile.close()If you need a different output, though, you will need to convert this agnostic G-code into a format suited for your machine. That is the job of post-processing scripts.
If you have a G-code file written for a particular machine, which doesn't comply to the internal rules used by FreeCAD, described in the "FreeCAD's internal G-code format" section above, it might fail to import and/or render properly in the 3D view. To remedy to this, you must use a pre-processing script, which will convert from your machine-specific format to the FreeCAD format.
If you know the name of the pre-processing script to use, you can import your file using it, from the Python console like this:
import example_pre
example_pre.insert("/path/to/myfile.ncc","DocumentName")In the same manner, you can output a Path object to G-code, using a post_processor script like this:
import example_post
example_post.export (myObjectName,"/path/to/outputFile.ncc")Pre- and post-processing scripts behave like other common FreeCAD imports/exporters. When choosing a pre/post processing script from the dialog, the import/export process will be redirected to the specified given script. Preprocessing scripts must contain at least the following methods open(filename) and insert(filename,docname). Postprocessing scripts need to implement export(objectslist,filename).
Scripts are placed into either the Mod/Path/PathScripts folder or the user's macro path directory. You can give them any name you like but by convention, and to be picked by the GUI dialog, pre-processing scripts names must end with "_pre", post-processing scripts with "_post" (make sure to use the underscore, not the hyphen, otherwise Python cannot import it). This is an example of a very, very simple preprocessor. More complex examples are found in the Mod/Path/PathScripts folder:
def open(filename):
gfile = __builtins__.open(filename)
inputstring = gfile.read()
# the whole gcode program will come in as one string,
# for example: "G0 X1 Y1\nG1 X2 Y2"
output = ""
# we add a comment
output += "(This is my first parsed output!)\n"
# we split the input string by lines
lines = inputstring.split("\n")
for line in lines:
output += line
# we must insert the "end of line" character again
# because the split removed it
output += "\n"
# another comment
output += "(End of program)"
import Path
p = Path.Path(output)
myPath = FreeCAD.ActiveDocument.addObject("Path::Feature","Import")
myPath.Path = p
FreeCAD.ActiveDocument.recompute()Pre- and post-processors work exactly the same way. They just do the contrary: The pre scripts convert from specific G-code to FreeCAD's "agnostic" G-code, while post scripts convert from FreeCAD's "agnostic" G-code to machine-specific G-code.
This example is based on a discussion in the german forum.
- Create a solid with ShapeString as Cutout
- Create a Job using this solid as its BaseObject
- Create a ProfileFromFaces operation named "Profile_Faces" with empty BaseGeometry.
The following code will then add all faces from ShapeString and create the paths:
doc = App.ActiveDocument
list_of_all_element_faces = []
for i, face in enumerate(doc.ShapeString.Shape.Faces):
list_of_all_element_faces.append('Face' + str(i + 1))
doc.Profile_Faces.Base = [(doc.ShapeString, tuple(list_of_all_element_faces))]
doc.recompute(){{Path_Tools_navi}}
⏵ documentation index > [Developer Documentation](Category_Developer Documentation.md) > [Python Code](Category_Python Code.md) > Path > Path scripting