Sunday, September 25, 2011

Engine: 4 - camshaft

Open model file with cams. Save it with different name, eg. camshaft.fcstd. Next select Part Design Workbench in Combo Select or by menu View-Workbench-Part Design.

You need revolve around Z-axis. Create new sketch on the XZ plane. You can also toggle visibility of cams by selecting one in Tree view and pressing [Space].
First end of shaft should be moved by 95. I recommend you sketching in steps: draw poliline with 3-4 segments, constrain they, then add next poliline. The shaft looks like a fusion of several cylinders:

Length Radius
20 8
23 10
30 12.5
72 10
16 12.5
70 10
2 13.5
16 12.5
2 13.5
70 10
16 12.5
72 10
16 12.5

In the left corner you can see a new feature in FreeCAD information about number of missing constraints or text Fully constrained sketch.

Close the sketch, and revolve it around Z-axis. You can set different angle but it this example 360 deg is necessary.

Unhide all shapes with [Space].

Boolean operations

Boolean operations are available in the Part workbench. Select the Part workbench. Next select all shapes with [Ctrl] key and click on "Make a union of several shapes" icon.

Now you have a new shape "Fuse". Return to the Part Design workbench. Select edges with [Ctrl] to fillet. Apply fillet and change it radius to 2 in Property view-Data.


Currently FreeCAD has very limited blueprints support.
Open Drawing workbench. Click on "Insert new drawing". Select a shape in Tree view and click on "Insert a new view of a Part in the active drawing". In a new tab you can see badly placed view. Tune placement in the Property view-Data-Drawing and Property view-Data-Shape view (in the Tree view Page-View have to be selected). In the screenshot you can see two views:
  • scale=0.5, x=100, y=100, direction x=0, y=0, z=1
  • scale=0.5, x=300, y=100, direction x=1, y=0, z=0
Finally you can export a page by clicking "Export a page to an SVG file" icon.

Download file.

Download first RAW Video.

Download second RAW Video.

FreeCAD 0.12 4957 SVN

Saturday, September 17, 2011

Engine: 3 - cams

Simple 8-valve engine needs only one camshaft: with 4 inlet and 4 exhaust cams. Today I'll design only cams - not entire camshaft.

Open a new sketch.

Our shape will be rotated by 14.24 deg. It is result of specified valves timing. Lets draw two connected lines: one horizontal, second rotated by 14.24 deg. Set second line length to 21.5. Next set they construction mode.

Construction lines are blue instead white. At the end set connecting point to (0, 0) with a lock constrain.
I need harmonic cam working with flat-faced follower. It can be constructed from four tangent arcs.
Take look at 21.5 mm line: left end will be bigger arc centre, right is for smaller arc centre. Draw arcs as in the above picture.

Now I should connect those arcs with two next, tangent arcs... but current (4928 SVN) FreCAD have not arc-arc tangency support. I drew two short, tangent for arcs, construction lines.

Next I connected arcs with second two (big radius ~100) ones. One of them I made tangent to two short construction lines. Additionally I set up first two arcs radius to 14 and 1.5 mm respectively. Connecting arcs should be exactly the same - use equality  constraint for them and next set two points (one end of each one) symmetrical for 21.5 mm line.
Note: also radius of connecting arcs should be specified but I have problems with this in 4928 SVN FreeCAD. I'll return to this issue in the future... 

Now you can make 12 mm pad. If shape isn't solid, check construction lines in the sketch.

Next I made second cam. This time shape is rotated by 167 deg from vertical line.

Now we have two cams: exhaust (first one) and inlet.

Select second cam and set Placement in Property view - Data. Set Z translation to -40.

For your convenience set names for Pads - click on it and press [F2]. Different colors also are useful - set they in Property view - View - Shape Color.

Now you can add next 6 cams: simply use Copy-Paste and Placement options.
Cam Z translation [mm] Rotation around Z axis [deg]
Exhaust 0 0
Inlet 40 0
I 88 90
E 128 90
E 176 270
I 216 270
I 264 180
E 304 180

And the final result:

Download model file.

FreeCAD 0.12 4928 SVN

Sunday, September 11, 2011

Engine: 2 - cylinder liner

In the simplest situation cylinder liner is a tube. I'll try design something more complicated.

Start FreeCAD, open Part Design workbench. You need section sketch which will be revolved around Y axis. Start a new sketch, and try create sketch like in the screenshot. The height is 137 and inner radius is 37.5. Use poliline and horizontal, vertical, coincident constraints. If any constraint is not necessary, click on it's icon and press [del].
Note: grid is useful, set grid to 10 mm (without snapping) in TaskView. FreeCAD shows you actual position near cursor.
Use lock constraint to fix sketch certain position (inner liner radius is 37,5).

Wall thickness is variable:
Distance from top Wall thickness
0 8
7 jump from 8 to 6
105 jump from 8 to 3
137 3

Close the sketch and make a revolution around Y axis.

To achieve minimal engine length we need cut some material from liner. Select a top face of liner and start sketching.

Draw two big rectangles symmetrical to Z axis. You can use a construction line (like in the "Pin ring tutorial") as centreline. Distance between rectangles is 88.
Finish editing the sketch and use a pocket tool.

Set (in Property View-Data) Pocket length to 137.

The final effect:
Download file.

Download RAW Video.

FreeCAD 0.12 r4907 SVN.

Saturday, September 3, 2011

Engine: 1 - piston pin and pin ring

Today I modelled two parts: pin connecting piston and conrod and ring locking axial move of that pin.

 Piston pin

Time 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":
x 1,00
y 0,00
z 0,00
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!

Download file.

Pin ring

Create 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.

Download file.
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


With this blog I'm going to deliver tutorial for application FreeCAD. FreeCAD tutorial blog is unofficial, I'm a normal FreeCAD user - not developer or  other superhuman:)

I'll  build combustion engine in this software. I promised it in this thread. The effect should be similar to:

  • 1-2 parts in almost every weekend,
  • simple parts (screws, valves, camshaft) first,
  • complicated parts (conrod, crankshaft, head) when PartDesign module gets sweeps, angle draft etc. features, 
  • blueprints - when Drawing module will be more mature,
  • and at the end: assembly,
  • optional: FEM, kinematics
If you don't know how FreeCAD looks like I would recommend you Youtube playlist:

To follow tutorials you need actual FreeCAD version. I'll write version at the end of each post.