FreeCAD Basic Exercise #1
The objective of this tutorial will be to discover the workflow for the parametric design of a 3D object with Part Design and Sketcher. For this we will model a basic part involving different types of functions.
Step 1: Presentation of the exercise
We will model the part illustrated below by the method proposed in the tree structure.
For the dimensions of the part you can refer to the drawing below but they will be repeated in the instructions.
This exercise allows the FreeCAD beginner to become familiar with the following workflow:
1. Creating a new sketch ;
2. Creating a closed contour with dimensional and geometric constraints;
3. Application of a modelling function to the previously created sketch.
Step 2: Creation of a first sketch
1.1. To start a new part design project, go to the Part Design workshop and create a new document (Ctrl + N).
1.2 In the toolbar, select "Create New Sketch", select the XY plane and then "OK". The interface then switches to the Sketcher workbench in Sketch Edit mode and the software automatically creates a Body which contains a marker and your new sketch (see Combined View - Model tab on the left of the screen).
1.3. In the toolbar, select the Rectangle tool then click anywhere in your main view, stretch the rectangle then click again. Deactivate the tool with Escape or with a right click.
1.4. Select the verticality icon associated with the left segment of the rectangle (the icon turns green) and then delete with the Delete key or (less quickly) with a right click → Delete after having located it in the combined view. The segment is no longer constrained in verticality.
1.5. Create a coincidence constraint (C) between the end of the rectangle and the origin of the frame.
1.6. Create 3 dimensional constraints as below with the horizontal distance (Shift + H) and vertical distance (Shift + V) or dimensional (Shift + D) functions only. The sketch is fully constrained and the outline appears in green.
Step 3: Adding 3D volumes
2.1. Exit the sketch (Escape) and use the Pad function to extrude your 20mm sketch.
2.2. Select the top of your part (which is highlighted) and then use the "Create new sketch" function to draw the outline below on your face. When creating your new rectangle, you can click directly on the origin of the marker to snap it.
2.3. Use the Pad function to extrude the 90 mm sketch.
Step 4: 3D volume subtraction
3.1 Create a new sketch on the newly created face.
3.2. Use the Circle and Dimensions functions to create the sketch below and then exit the sketch (Escape).
3.3. Use the Pocket function to drill from the created sketch, set the Type parameter to "Through All".
Step 5: Dress-up
4.1. Use the Fillet function to round the edge of your piece.
Step 6: Transformation tools
5.1. Select your part Body
5.2. Activate the Mirrored tool and select all the elements of the tree structure (functions) previously created.
5.3. Click on OK to validate the selection of the elements and then on OK again to validate the selection of the symmetry plane.