FreeCAD: Solid Modeling with the power of Python with this book and ebook.

For most casual users, the stable version binaries are the best place to start learning FreeCAD.

Start by visiting the FreeCAD site at http://free-cad.sourceforge.net/.

The main page of the FreeCAD site has a panel with download links for the current stable release.

The 3D area allows you to see and navigate around your design in space.

The combo view shows a hierarchical view of the project or the state of the current task.

The tool bars and workbench switcher gives access to the various tools.

Open a new document by clicking on the menu File | New. The 3D view will switch to show an empty space. In the default orientation the camera position is looking down onto a plane defined by the X and Y axes. The Z axis is pointed directly at the camera. A coordinate indicator in the corner helps you orient yourself in the 3D space.

Click on the workbench switcher and select the Part workbench. Then click on the Create a box solid icon to insert a cube into the project.

You can have multiple projects open at the same time. You can also open multiple views of the same project. Open a second view of the project by clicking on the menu View | Create new view. You can switch views with the tabs below the 3D window or you can tile the views to have multiple perspectives at once. In this following screenshot, two projects are open, each with two views:

You can change the view of your project by panning, rotating, and zooming. Select objects by clicking on them to change their properties. The specific mouse and keyboard commands for doing this are called "navigation styles". FreeCAD supports four styles by default: Inventor, CAD, Blender, and Touchpad.

You can change the style used in the current view by right-clicking on the 3D canvas.

Changing the style through the Edit | Preferences menu will change the style for all views currently open and set the selection as the default for new views. The default style, CAD navigation, is unintuitive for some users since it requires clicking both the left and center mouse buttons at the same time to rotate. The Mouse... button in the Display preferences will show which button combinations perform each action.

Select the box and tap the space bar to toggle the object visibility property. Visibility is one of many properties of any object on screen. With the box still selected, examine the lower part of the combo-view. The properties of the selected object are shown on the two tabs (View and Data).

Click on the Measure distance icon, and then click two points on the box in the 3D window. A dimension will be shown and a distance object will be added to the tree.

You can select the distance object in the tree and explore its properties.

As the project complexity grows, you may need to perform an action on multiple objects at the same time. Select multiple objects by holding the Ctrl key while selecting with the mouse.

Model the bent metal plate by adding and positioning three box solids. Add the first box to the drawing, and select its node in the project tree. Switch to the Data tab and edit the properties to make it 2.5 x 50 x 50 mm (height, length, width).

Create a second box with the same dimensions but edit the placement to move the box 50 mm in the X direction and 10 mm in the Z direction. This will place the second cube next to the first and shifted upward.

Add a third cube to connect them. Make its dimensions 10 x 2.5 x 50 mm and shift its placement 50 mm in the X direction.

If you rotate your view slightly, your three solids should look like the following figure:

Next we'll create the slots. FreeCAD doesn't have a slot feature so we'll make a solid in the shape of the hole we want. Later, we'll subtract it from the plate to create the hole.

Add another box and set its dimensions to 10 x 10 x 3 mm.

We want the slot to have rounded ends so we will fillet the box. Select the box and press the menu Part | Fillet.

The combo view will switch to the Tasks panel and show the fillet options. You can use this to refine your edge selection and set the radius of the fillet. For our example, select Edge1, Edge3, Edge5, and Edge7. We used a value of 1 for the radius. Clicking on the OK button will apply the change. If you make a mistake, double-click the fillet object in the tree to change the properties and try again.

Once the cube looks right, select it and duplicate it with the menu item Edit | Duplicate selection. Repeat this twice more so that we have a total of four fillet objects. Select each one and change its placement properties to move it into position on the raised part of the plate. The position is up to you. Just make sure the fillet objects completely penetrate the plate.

Now add five cylinders for the holes. Change their placement and radius properties. The center hole is 22.5 mm and the small screw holes are 2.5 mm.

With all the solids added to the project, it should like the following image:

We're almost ready to subtract the cylinders and slots from our base plate, but we first need to clean things up a bit. In the project tree, select all of the cylinders and fillet objects. With all of them selected, click on the Make a union of several shapes icon:

Now select the three boxes for our base plate and repeat the operation, fusing them into a single object.

You should now have two fusion objects in the tree, one for the base plate and one for the holes that will be cut from it. First select the base plate fusion, and then with Ctrl held down, select the other. Click on the Make a cut of two shapes icon:

The order in which you select the objects is important. The first object will be cut by the second. If all goes well, you will have an object that looks almost like the image at the beginning of the recipe.

To finish it off, we've applied another round of fillets to the corners of the plate and to the corners of the bend. The complete object should look like the image at the beginning of this recipe.

Press the red record button shown in the following screenshot:

The macro recording dialog box will pop up. Give your macro a name and save it:

Perform the tasks that you want recorded. You can create a macro of whatever you normally do in FreeCAD. Macros that deal with simple part creation are easiest to start with. Try creating a box in the Part workbench and change its width to 20 mm.

When you are done recording the tasks, press the green button to stop recording:

Run your macro by selecting the button that looks like a sketch pad:

Select the name of the macro that you created and click on Execute:

Select the wire tool. Deselect the Relative checkbox. Points of a wire can be added by clicking the canvas or manually by keying in coordinates. Manually enter the first point at X = 3.175, Y = -5, and Z = 0. You can Tab from field to field and hit Enter on Z to create the point.

Continue adding a second point at X = 3.175, Y = 10, Z = -0.

Enter the remaining points working clockwise around until your wire looks like the following image. The remaining points can be added by clicking the canvas, and snapping to the grid if you prefer. Holding the Shift key will force new segments to be orthogonal.

Before we can edit any part of the wire we have to explode it into a collection of edges. Select the wire in the project tree. Select the Draft menu and click on the Downgrade button three times.

We'll replace the square edge of the rim with a arc. Make sure that midpoint and endpoint are enabled on the snapping toolbar. Use the arc tool and draw a curve on the rim.

Repeat for the other rim, then delete the old straight edges.

Select all the edges in the tree. Select the Draft menu and click on the Upgrade button to rejoin them into a wire.

Switch to the Draft workbench.

Select the wire and click on the Upgrade button to convert it to a face.

Switch to the Part workbench.

Press the Revoke a selected shape button:

In the Revolve dialog, select the shape to rotate.

Select the axis around which to revolve. For our example, use the Y axis. Leave the other settings unchanged and click on OK.

The revolved object is added to the project.

Enter the following text into the Python console:

import Part
from FreeCAD import Vector

plate = Part.makeBox(40,40,5,Vector(-20,-20,0))
hole1= Part.makeCylinder(1.5,5,Vector(-15,-15,0))
hole2= Part.makeCylinder(1.5,5,Vector(-15,15,0))
hole3= Part.makeCylinder(1.5,5,Vector(15,15,0))
hole4= Part.makeCylinder(1.5,5,Vector(15,-15,0))
faceplate = plate.cut(hole1)
faceplate = faceplate.cut(hole2)
faceplate = faceplate.cut(hole3)
faceplate = faceplate.cut(hole4)
motorbody=Part.makeCylinder(17.5,60,Vector(0,0,5))
shaft = Part.makeCylinder(3.175,15,Vector(0,0,-15))
servo = motorbody.fuse(faceplate)
servo = servo.fuse(shaft)
servo.translate(Vector(-20,-20,0))
servo.rotate(Vector(0,0,0),Vector(0,1,0),-90)
Part.show(servo)

Make sure to press the Enter key after the last line.

You should see a 3D solid in the graphics screen of FreeCAD that looks similar to the following graphic:

Type the following code into the Python console exactly as shown. Python is case and indent sensitive. Be consistent on indentation. We will use four spaces per indent here. An intent looks like a tab in this text. I have added \ (backslashes) to some lines that won't fit on the printed page in their complete form.

from PyQt4 import QtGui,QtCore
import Part,FreeCAD
from FreeCAD import Base,Vector

class BoxExample(QtGui.QWidget):
    def __init__(self):
        super(BoxExample, self).__init__()
        self.initUI()
    def initUI(self):
        self.setGeometry(100, 100,300, 200)
        self.setWindowTitle('Make a Box!')
        self.lengthLabel = QtGui.QLabel("Length: ",self)
        self.lengthLabel.move(50, 15)
        self.length = QtGui.QLineEdit(self)
        self.length.move(100, 15)
        self.widthLabel = QtGui.QLabel("Width: ",self)
        self.widthLabel.move(50, 50)
        self.width = QtGui.QLineEdit(self)
        self.width.move(100, 50)
        self.heightLabel = QtGui.QLabel("Height: ",self)
        self.heightLabel.move(50, 85)
        self.height = QtGui.QLineEdit(self)
        self.height.move(100, 85)
        self.centered=QtGui.QCheckBox("Center on XY",self)
        self.centered.move(80, 115)
        self.centerbox = False
        self.centered.stateChanged.connect(self.changeState)
        self.okButton = QtGui.QPushButton("Create Box",self)
        self.okButton.move(160, 150)
        self.show()
        QtCore.QObject.connect \
(self.okButton, QtCore.SIGNAL("pressed()"),self.box)  
    def changeState(self, state):
        console=FreeCAD.Console
        if state == QtCore.Qt.Checked:
            console.PrintMessage("Box will be centered\n")
            self.centerbox = True
        else:
            self.centerbox = False
    def box(self):
        l = float(self.length.text())
        w = float(self.width.text())
        h = float(self.height.text())
        if self.centerbox == True:
            box = Part.makeBox(l,w,h)
            box.translate(Base.Vector(-l/2,-w/2,0))
        else:
            box = Part.makeBox(l,w,h)
        Part.show(box)

d = BoxExample() 

Press the Enter key twice after typing in the last line.

When the dialog box pops up, fill in the values and click on the Create Box button. A simple 3D box should appear in the FreeCAD document. It looks similar to the following screenshot:

Roughly draw the end profile of the part. Don't worry about accuracy at this point. The following example was drawn with an arc and a wire:

Add geometric constraints. Constraints are added by selecting the parts of the sketch to be constrained and pressing the appropriate constraint button. A new constraint icon will be added to the drawing and it will be listed in the left-side panel.

Start by adding horizontal and vertical constraints to any crooked lines.

If lines are supposed to connect, select the vertexes and add coincident constraints.

Select pairs of matching lines and add an equality constraint. This forces the lines to be equal length.

When the sketch looks symmetrical, add dimension constraints. Start by constraining the most important dimensions. For instance, we've constrained the radius of the arc to 25 mm.

As you add constraints, watch the solver message at the top of the task panel. As the number of Degrees Of Freedom (DOF) approaches zero you may find it difficult to add constraints without getting a conflicting constraints error. Grabbing a vertex or segment and dragging it can show you where the sketch is still under constrained.

If the sketch gets to 2 DOF and dragging a segment just moves the entire sketch, it's time to lock it. Pick a vertex (we used the center of the arc) and click on the lock button. This will add vertical and horizontal distance constraints which lock the vertex to the origin of the coordinate system. A fully constrained sketch will turn green. Celebrate.

Click on the close button in the task panel. Use the pad tool to pad the sketch to 75 mm and rotate the sketch to see your part.

Even after the sketch has been padded, you can still edit it by double-clicking it in the tree. When saved, your changes will be immediately incorporated into the part.

Select the top face of the part so it is highlighted and click on the sketch button. The new sketch will be mapped to the face.

Draw four circles to represent our bolt holes. Select all four by clicking the edge (not the center) and set an equality constraint so they're the same size.

Select one of the four and add a radius constraint. Set the radius to 3.5 mm. Now all four can be resized by changing one number.

We want the holes to be positioned symmetrically. Select the centers of the top two holes and the vertical axis. Add a symmetry constraint. Repeat for the bottom two holes. The two sets of circles are now independently symmetrical.

Draw a line from the center of the top-right hole to the center of the bottom-right hole. Make sure the end points are coincident with the center of each circle. Select the line and make it into a construction line by clicking on the construction mode icon.

Set a length constraint on the construction line of 50 mm.

Now we need a way to set the position of the holes relative to the edge of the part.

Click on the External Constraint icon and select the right edge of the original solid. The edge and its vertexes can now be referenced in constraints as though they were a part of the sketch.

Select the center of the bottom-right circle and the bottom-end point of the external constraint line. Add a horizontal distance constraint (11 mm). Repeat and add a vertical distance constraint (15 mm).

The sketch should be fully constrained. To create holes all the way through the block, close the sketch and use the pocket tool. Set the pocket depth to at least 50 mm.

Enter the following code block into the console:

from Sketcher import *  
import Part
import FreeCAD as App
from FreeCAD import Vector
if(App.activeDocument() == None):App.newDocument()

f = App.activeDocument().addObject("Sketcher::SketchObject",\"Sketch")
f.addGeometry(Part.Line(Vector(0,0,0),Vector(2,20,0)))
f.addGeometry(Part.Line(Vector(0,0,0),Vector(20,2,0)))
f.Constraints = [Constraint('Vertical',0),\Constraint('Horizontal',1)]
App.activeDocument().recompute()

Double-click on the Sketch icon in the Project tree.

Notice the horizontal and vertical constraint symbols (the small red bars). Also notice that the lines have end points but they aren't constrained.

Grab either of the lines and move it and the other one won't move with it.

Add some more Python code to the console to constrain some points:

StartPoint = 1 ;
l = f.Constraints
l.append(Constraint('Coincident',0,StartPoint,1,StartPoint))
f.Constraints = l
App.activeDocument().recompute()

Notice how one end of each line has connected to the other.

Try moving one of the lines around the screen and you will see that the lines move together.

Import all available functions in the Sketcher module:

from Sketcher import *  

We will need the Part module to make geometric objects:

import Part  

The FreeCAD module will let us manipulate the document:

import FreeCAD as App  

We will need to give our line segments end points, so we need:

from FreeCAD import Vector

If a document isn't already open create a new one:

if(App.activeDocument() == None): App.newDocument()

Create a new Sketch object:

f = App.activeDocument().addObject("Sketcher::SketchObject",\"Sketch")

Add geometry to the sketch:

f.addGeometry(Part.Line(Vector(0,0,0),Vector(2,20,0)))
f.addGeometry(Part.Line(Vector(0,0,0),Vector(20,2,0)))

Add some constraints to the sketch to make the lines horizontal and vertical:

f.Constraints = [Constraint('Vertical',0),\Constraint('Horizontal',1)]

Recompute the sketch to see things after changes:

App.activeDocument().recompute()

Let's add a name for startpoints on our lines:

StartPoint = 1

Create a proxy object that is equal to our original, because we cannot add constraints directly to it:

l = f.Constraints

Append more constraints to our proxy object. 0 is the first line and 1 is the second:

l.append(Constraint('Coincident',0,StartPoint,1,StartPoint))

Make the original constraints equal to the proxy and recompute:

f.Constraints = l
App.activeDocument().recompute()

Select the Insert new drawing icon:

Pick the Insert an orthographic projection icon:

A new task will pop up in the Task panel. Select a Primary View:

Select Secondary Views:

Click on the OK button in the Task panel.

While the Page icon is selected in the Project tree, click on its Data tab.

Double-click on the button that has ... as its label.

A text dialog box will popup. Edit the values, putting in your name, the date, and so on:

Click on the recompute button to see the results:

In the Project tree, select 2D geometry from a Sketch or the Draft workbench. Be sure and select all geometry that you want exported.

From the top menu, select File and then Export.

In the lower-right corner of the Export file dialog, select Autodesk DXF.

In the Name entry box, give your file a name with the *.dxf extension.

Select the directory where you want your file saved.

In FreeCAD, open the Draft workbench and then select Preferences from the Edit menu.

In the Preferences dialog, click on the Draft icon and then click on the Import/Export tab.

Under DXF format options, change Import style to None (fastest).

Uncheck all the other boxes in that same section. Click on Apply and then OK.

In FreeCAD, select Import from the File menu.

Select the dxf file that you want to import.

In the Combo View, look at the Project tab and expand the icons.

Switch to the Draft workbench so that we can Upgrade the Circle with the icon that looks like an arrow pointing upward.

Select the geometry labeled as Polyline and use the Part workbench with the Extrude icon to extrude it into a solid.

Extrude the geometry labeled Circle into a solid. Make sure that its height is the same as the solid made from Polyline.

Select the solid that you created from Polyline and then the solid created by Circle.

Use the Boolean Cut operation in Part workbench to subtract the Circle solid from the Polyline solid.