PartDesign tutorial/en

Introduction
This tutorial is meant to introduce the reader to the basic workflow of the PartDesign Workbench.



Requirements

 * FreeCAD version 0.16 or above
 * The reader has read the Sketcher tutorial

Creating 3D geometry
The purpose of the PartDesign Workbench is to allow the user to create geometry in 3D space to fulfill a certain need. As such, it is equipped with tools to make use of sketches and convert them to 3D objects.

There are two basic features to achieve this: Pad and   Revolution. Alongside their subtractive counterparts ( Pocket and Groove) they make up most of the common actions used by this workbench.


 * 1) Switch to the PartDesign Workbench
 * 2) Select the sketch that was created in the Sketcher tutorial
 * 3) Select [[Image:PartDesign_Pad.png|32px]] Pad
 * 4) Set the distance to 5 mm
 * 5) Select Ok

Another way to create 3D geometry is with the  Revolution tool.




 * 1) Create a sketch based on the image above
 * 2) Select [[Image:PartDesign_Revolution.png|32px]] Revolution
 * 3) Set the angle to 360°

Subtracting Features
We'll begin by creating a sketch with the shape we want to subtract.


 * 1) Select the top face of the Pad
 * 2) Select [[Image:Sketcher_NewSketch.png‎‎|32px]] New sketch
 * 3) Select [[Image:Sketcher_External.png|32px]] External Geometry
 * 4) Approach the edge of the pad. An arc should be highlighted
 * 5) Select the arc. An arc of a different color should appear in the sketch
 * 6) Create a circle centered on the same point as the arc and set its radius to 5 mm



Afterwards, we'll proceed to apply a Pocket feature.


 * 1) Select the sketch
 * 2) Select [[Image:PartDesign_Pocket.png|32px]] Pocket
 * 3) Set the distance to Through all

Pattern Features

 * 1) Select the top face of the object
 * 2) Create a new Sketch
 * 3) Create reference geometry linked to the top arm of the figure
 * 4) Create a circle constrained to the center of the reference arc
 * 5) Set its radius to 3 mm
 * 6) Pocket the sketch through all the workpiece

Instead of creating a circle for each hole in the sketch, we will introduce the concept of Pattern Features. These tools operate by replicating a feature in the workpiece that has already been created and that we wish to reproduce in a linear or circular arrangement. We will use a combination of Linear and Polar pattern features simulatneously to obtain the final workpiece.


 * 1) Select the Pockt feature that we just created in the Tree View
 * 2) Select [[Image:PartDesign_MultiTransform.png|32px]] MultiTransform

In the Combo View we are now asked to introduce the Transformations that we desire. Notice that in the MultiTransform parameters menu we see that FreeCAD has identified the Pocket as the Original feature and a second box requests us to Right click it to introduce the pattern features.


 * 1) Right click the box
 * 2) Select Add Linear Pattern
 * 3) Set the Direction to Vertical Sketch Axis
 * 4) Set length to 10 mm
 * 5) Leave occurrences at 2
 * 6) Click OK
 * 7) Right click the box again to add a Polar Pattern. Notice that the 3D view has now added the linear pattern.
 * 8) Set occurrences to 5
 * 9) Click OK twice

After completing this task you should have the following result.



If not, re-edit the MultiTransform operation by double clicking on it in the Tree View. Check both pattern features to detect necessary modifications, such as the Axis and if the Direction needs to be reversed.

We are now finished with the basic workflow for the Sketcher Module.