# Manual:Creating and manipulating geometry

- Introduction
- Discovering FreeCAD
- Working with FreeCAD
- Python scripting
- The community

In the previous chapters, we learned about the different workbenches of FreeCAD, and how each of them implement their own tools and geometry types. The same concept applies when working from Python code.

We also saw that the vast majority of FreeCAD workbenches depend on a very fundamental one: the Part Workbench. In fact, many other workbenches, such as Draft and Arch, do exactly what we will do in this chapter: use Python code to create and manipulate Part geometry.

So the first thing we need to do to work with Part geometry, is to do the Python equivalent to switching to the Part Workbench: import the Part module:

```
import Part
```

Take a minute to explore the contents of the Part module, by typing Part. and browsing through the different methods available. The Part module offers several convenience functions such as makeBox, makeCircle, etc... which will instantly build an object for you. Try this, for example:

```
Part.makeBox(3,5,7)
```

When you press Enter after typing the line above, nothing will appear in the 3D view, but something like this will be printed on the Python Console:

```
<Solid object at 0x5f43600>
```

This is where an important concept takes place. What we created here is a Part Shape. It is not a FreeCAD document object (yet). In FreeCAD, objects and their geometry are independent. Think of a FreeCAD document object as a container, that will host a shape. Parametric objects will also have properties such as Length and Width, and will **recalculate** their Shape on-the-fly, whenever one of the properties changes. What we did here is calculate a shape manually.

We can now easily create a "generic" document object in the current document (make sure you have at least one new document open), and give it a box shape like the one we just made:

```
boxShape = Part.makeBox(3,5,7)
myObj = FreeCAD.ActiveDocument.addObject("Part::Feature","MyNewBox")
myObj.Shape = boxShape
FreeCAD.ActiveDocument.recompute()
```

Note how we handled myObj.Shape , notice that it is done exactly like we did it in the previous chapter, when we changed other properties of an object, such as box.Height = 5 . In fact, **Shape** is also a property, just like **Height**. Only it takes a Part Shape, not a number. In the next chapter we will have a better look at how these parametric objects are constructed.

For now, let's explore our Part Shapes in more detail. At the end of the chapter about traditional modeling with the Part Workbench we showed a table that explains how Part Shapes are constructed, and their different components (Vertices, edges, faces, etc). The exact same components exist here and can be retrieved from Python. Part Shapes always have the following attributes: Vertexes, Edges, Wires, Faces, Shells and Solids. All of them are lists, that can contain any number of elements or be empty:

```
print(boxShape.Vertexes)
print(boxShape.Edges)
print(boxShape.Wires)
print(boxShape.Faces)
print(boxShape.Shells)
print(boxShape.Solids)
```

For example, let's find the area of each face of our box shape above:

```
for f in boxShape.Faces:
print(f.Area)
```

Or, for each edge, its start point and end point:

```
for e in boxShape.Edges:
print("New edge")
print("Start point:")
print(e.Vertexes[0].Point)
print("End point:")
print(e.Vertexes[1].Point)
```

As you see, if our boxShape has a "Vertexes" attribute, each Edge of the boxShape also has a "Vertexes" attribute. As we can expect, the boxShape will have 8 vertices, while the edge will only have 2, which are both part of the list of 8.

We can always check what is the type of a shape:

```
print(boxShape.ShapeType)
print(boxShape.Faces[0].ShapeType)
print(boxShape.Vertexes[2].ShapeType)
```

So to resume the topic of Part Shapes: Everything starts with Vertices. With one or two vertices, you form an Edge (full circles have only one vertex). With one or more Edges, you form a Wire. With one or more closed Wires, you form a Face (the additional Wires become "holes" in the Face). With one or more Faces, you form a Shell. When a Shell is fully closed (watertight), you can form a Solid from it. And finally, you can join any number of Shapes of any types together, which is then called a Compound.

We can now try creating complex shapes from scratch, by constructing all their components one by one. For example, let's try to create a volume like this:

We will start by creating a planar shape like this:

First, let's create the four base points:

```
V1 = FreeCAD.Vector(0,10,0)
V2 = FreeCAD.Vector(30,10,0)
V3 = FreeCAD.Vector(30,-10,0)
V4 = FreeCAD.Vector(0,-10,0)
```

Then we can create the two linear segments:

```
L1 = Part.LineSegment(V1,V2)
L2 = Part.LineSegment(V4,V3)
```

Note that we didn't need to create Vertices. We could immediately create Part.LineSegments from FreeCAD Vectors. This is because here we haven't created Edges yet. A Part.LineSegment (as well as Part.Circle, Part.Arc, Part.Ellipse or Part.BSpline) does not create an Edge, but rather a base geometry on which an Edge will be created. Edges are always made from such a base geometry, which is stored in its Curve attribute. So if you have an Edge, doing:

```
print(Edge.Curve)
```

will show you what kind of Edge it is, i.e. if it's based on a line, an arc, etc... But let's come back to our exercise, and build the arc segments. For this, we will need a third point, so we can use the convenient Part.Arc, which takes 3 points:

```
VC1 = FreeCAD.Vector(-10,0,0)
C1 = Part.Arc(V1,VC1,V4)
VC2 = FreeCAD.Vector(40,0,0)
C2 = Part.Arc(V2,VC2,V3)
```

Now we have 2 lines (L1 and L2) and 2 arcs (C1 and C2). We need to turn them into edges:

```
E1 = Part.Edge(L1)
E2 = Part.Edge(L2)
E3 = Part.Edge(C1)
E4 = Part.Edge(C2)
```

Alternatively, base geometries also have a toShape() function that do exactly the same thing:

```
E1 = L1.toShape()
E2 = L2.toShape()
...
```

Once we have a series of Edges, we can now form a Wire, by giving it a list of Edges. We do need to take care of the order.

```
W = Part.Wire([E1,E4,E2,E3])
```

And we can check if our Wire was correctly understood, and that it is correctly closed:

```
print( W.isClosed() )
```

Which will print "True" or "False". In order to make a Face, we need closed Wires, so it is always a good idea to check that before creating the Face. Now we can create a Face, by giving it a single Wire (or a list of Wires if we want holes):

```
F = Part.Face(W)
```

Then we extrude it:

```
P = F.extrude(FreeCAD.Vector(0,0,10))
```

Note that P is already a Solid:

```
print(P.ShapeType)
```

This is because when we extrude a single Face, we always get a Solid. This wouldn't be the case, for example, if we had extruded the Wire instead:

```
S = W.extrude(FreeCAD.Vector(0,0,10))
print(s.ShapeType)
```

Which will of course give us a hollow shell, with the top and bottom faces missing.

Now that we have our final Shape, we are anxious to see it on screen! So let's create a generic object, and assign our new Solid to it:

```
myObj2 = FreeCAD.ActiveDocument.addObject("Part::Feature","My_Strange_Solid")
myObj2.Shape = P
FreeCAD.ActiveDocument.recompute()
```

Alternatively, the Part module also provides a shortcut that does the above operation quicker (but you cannot choose the name of the object):

```
Part.show(P)
```

All of the above, and much more, is explained in detail on the Part Scripting page, together with examples.

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