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

FreeCAD 0.12 4928 SVN

Thanks for this tutorial. It seems to me that there is still no arc-arc tangency support in 0.13 version (4972 Launchpad), though no error is displayed after selecting to arcs and then click Create a tangency constraint icon.

ReplyDeleteAdding sound would be very helpful. What could have been a good learning tool

ReplyDeleteturn into ? .

I think I got the arc-arc tangency working (latest daily), but setting the radius of the big arcs seems to fail, complains about conflicting constrains after stalling for a while.

ReplyDeletearc to arc tangent works for me with 0.13 Rev 1828. It becomes easy enough to do if initially the centers of the arcs are near their final positions.

ReplyDeleteI'm having some trouble editing the placement of the second cam. In the property/data window I can edit the lengths of the pad but not the placement (either position or orientation). Is there something I'm missing?

ReplyDeleteOn another note, thanks for an excellent set of tutorials! Has really helped me get used to working with a new CAD package.

Part Design features behaviour has been changed due to compatibility with upcoming Assembly workbench. You cannot change a Pad placement any more.

ReplyDeleteWorkaround: use the Extrude tool from the Part Workbench instead.

Works like a dream, thanks very much!

ReplyDeleteVery nice tutorial. Thanks for taking the trouble!

ReplyDeleteYou write above: Next I connected arcs with second two (big radius ~100) ones. One of them I made tangent to two short construction lines.

How did you connect these arc to the end points of the two other arcs? Unless you get the exact point at which to place the center of the arc, you cannot "stretch" the arc to intersect with the two end points. Am I missing something?