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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.

Blueprints

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

3 comments:

  1. Having chosen to create the new sketch on the XZ plane, as said in the tutorial, and after having sketched the camshaft, I was unable to revolve it around Z-axis. Only "horizontal" (around X) or "vertical" (around Y) were possible using the sketch revolution tool. Even from the Project view, by selecting the new Revolution object, I was unable to change its axis data from (x, y, z) = (1, 0, 0) to (0, 0, 1).

    ReplyDelete
  2. I cancel my previous comment. That was a bug. Now it rotates around the good axis.

    ReplyDelete
  3. I upadted from 0.13 4972(Launchpad) to 0.13 25th of february 2012

    ReplyDelete