Piston pinTime to start FreeCAD...
FreeCAD start page is opened. Click on the Part Design link.
Now you are in Part Design Workbench. Click at the icon "Create a new Sketch" with circle and rectangle to start sketching.
You can see grid and two blue lines - 0X and 0Y axis. Red geometry icons became active, so click on rectangle icon and draw it. At this moment dimensions aren't important.
You have a rectangle. Try set up width: click on upper line and set constrain "Fix a length of a line...". Then you should see dimension. Double click on it and set to 60 millimetres. You can delete constraints by key [del]. In the left bottom corner there is "Task View" with list of used constraints.
Now we need smaller and bigger radius of our pin. Select one (bottom) point and use "Fix the vertical distance between two point or line ends". Only one point was selected, so it is distance from 0X axis.
Do exactly the same operation with second (upper) point and set dimensions to 6 and 11.
Now you can revolve sketch. Stop editing sketch by pressing "Close" button in "Task View" or icon "Close the editing of sketch". It is time to revolve by clicking icon "Revolve a selected sketch". Important: be sure that sketch is selected in "Tree view".
Houston, we have a problem. Sketch was revolved around Y-axis (coordinate system is in right bottom corner) but it should revolved around X-axis. Select Revolution in "Project view" and set values in "Data Tab":
Revolve should update - if not (bug in the application): activate sketch in "Tree view" (you can hide/unhide elements by [Space]) by double clicking on it and change something, eg. length constraint from 60 to 55. When you close editing sketch revolve will be updated.
Now you have pin. If you need chamfer edges, select tool "Chamfer the selected edges of the shape" (the revolution have to be selected before) and click on those edges.
List of selected edges are in "Task View"
Fillet works in a different way. Firstly you have to have selected edges, after clicking "Make fillet on an edge, face or body" fillets will be created. You can change radius of fillet in "Project view"-"Data" tab.
That's all, experiment yourself!
Pin ringCreate new file, Select Part Design workbench and create new sketch. Try draw vertical line - you should see small icon nearly cursor. It is autoconstraining: line become vertical automatically. Next select bottom point (end of line) and use "Create a lock constraint on the selected item".
You can see two dimensions started from point (0,0). Set they to 0 - line would be our centreline.
Draw arc: first is centre point, next points will determine start and end angle. Try set up centre on bottom end of line if you have problem with autoconstraining, use "Create a coincident constraint..." (red point icon). Next use "Fix the radius..." to set radius = 11.5.
Fix the horizontal distance between start point and centreline to -1,20 - select point and line before.
Create next arc higher, put it centre at centreline by "Fix a point onto an object" constraint and set vertical distance to 1.3.
Connect arcs with polilines. Next constrain left side with distance and angle constraints.
Left and right points have different position - we need something like a mirror. You can use symmetry constraint: select left point, right point and centreline then use "Create an symmetry constraint..."
Draw two circles. Set position one of them by "Create a lock..." 9.20 vertical and -3 horizontal would be good. Use symmetry constraint, and "Create an equality constraint...". At the end set the radius to 1.
Our sketch is complete but we have to do one important thing. Our "centreline" actually is a normal line. To not collide with sketch shape during Pad centreline must be toggled to construction mode - please select icon line with red points and blue line.
Click "Close the editing of the sketch" and next click "pad" in "Task View". At the end set pad length to 1mm in "Task View".
You can add also some fillets.
If you stuck somewhere during this tutorial you can download video.
What can you do with this model? For example:
- export as STEP file (select File-Export, part object have to be selected in Tree view),
- create 2D views and save it as SVG file (you can use Inkscape to convert SVG to DXF, FreeCAD DXF-exporter is still buggy),
- create a mesh.
Version of FreeCAD: 0.12 r4875 SVN