Class 43: the upper cabin, refined

The upper cabin is re-extruded, using the newly made lower valance top profile.


The shape is fine up to the real top dome: the diagonal ridge must be removed.
I decided to keep only the lower bulk of the cabin, cutting out the really curved top and the back straight part. This allowed me to focus on the top curved shape.

I realized it intersecting two parts of ellipsoids. The ridge at their intersection can be easily smoothed with the “fillet” tool of FreeCAD.

cap_pyramThis cap extends below the top of the cabin bulk, only the upper part is kept: a solid, shaped as a pyramid, with the faces sloping tangentially to the uppermost section of the bulk, is used to cut out the top cap.

The top and the bulk are properly matching at the sides. Extending the back face of both, the cabin shape is complete: only the spiky edge at the front of the bulk must be smoothed. This is easily done, cutting out the edge with a huge cone.

In the resulting shape there is no more mismatch between the top cap and the bulk. A fillet with a big radius on the cone-cutout right edge (in green in the picture), gives then the final shape. The back of the upper cabin is backwards extended horizontally to the required full length of the cabin.

Class 43 lower valance with FreeCAD

The basic lower valance is too prominent in the upper curved profile and too spiky in the lower part: a round cutout of the shape is needed. The right curve is created with an eight of an ellipsoid, placed and shaped with a fine tuning to match exactly the needed curve as well as the remaining parts of the basic shape.

The front part of the valance is then created extruding the side face of the ellipsoid, while the back side part of the basic valance is kept. With a little work of extrusion and boolean operations, the final lower valance full shape is there.

For the final cabin, an empty shape is needed, with a given thickness. It’s enough to clone (in green in the picture) the full shape, place it backwards and inwards of a distance equal to the needed thickness and cut it out from the original full shape.

Now the new top face of the lower valance must be extracted and used to make the upper cabin profile match the lower valance.

Class 43: once more

Time came to add the details to the class43 plain model. When trying to intersect one of the details with the lower valance, imported as stl object, the troubles came: FreeCAD doesn’t support stl proper handling and it was not really possible to do boolean operations between FreeCAD objects and and stl import. Perfectionist as I am, as well as my modelling partner is 😉 , I took the chance to re-think the cabin as a complete FreeCAD project. The basic shape is still created intersecting the extrusions of the three orthogonal profiles, this time created with Inkscape from the blueprint and imported directly into FreeCAD in  svg format.

The cabin is again split into two parts: the upper part and the lower valance.


Twisted gear easy made

Some time ago I struggled to build a twisted gear with the “loft” tool inside FreeCAD for the logo of our company.

There’s a much easier way: still inside FreeCAD the “sweep” tool used along a helix. It’s enough to draw a helix and sweep the face of the gear along it. gear_helixThe face (in grey) lays on the x-y plane and is centred around the z axis; the helix (in green) is also centered around the z axis. The helix is used as “sweep path” and the face is the object to be swept.

The only tgear_cubericky part to pay attention to is that the upper surface of the sweep solid will not be parallel to the base: it’s enough to have the helix’s height bigger than the height needed for the twisted gear and intersect the resulting twisted solid with a cuboid with the base larger than the gear face and the exact needed height.

The twisted gear is ready:




Swiss buffers: the design

Without any blueprint or measures, but only a collection of pictures, I used Inkscape to do some guesstimations of shapes and dimensions: I imported the digital photos and overlayed on the hand created rectangles and ellipses, adjusting my shapes until they met the original picture. I then extracted the dimensions of the shape objects and used them to design the buffer with FreeCAD. With the supervision my modeling partner expert’s eye, I did the final tuning.

Now it’s time to add the supports for the 3D print and replicate them in a matrix, ready to be printed.

A curved frame: solution two

fr_cutfr_cut2I tried a different approach to the 3D design challenge for the curved frame: create a set of full curved layers to build the geometry of the required circular section, to the extension of the frame, thencut it through in the middle with a cylinder sector.

Being symmetrical, it’s enough to build a quarter of the frame and then mirror it. The required frame section must be sliced in three layers, corresponding to the horizontal lines in the picture above. Each layer is as long as half of the straight side length and must be swept along the curved side of the frame. All the sweeps start from the middle of the curved side, on one of the reference planes (I choose the x-z plane for the sketch and the x axis for the revolution), where the two symmetric parts of the final frame will be attached together. The geometrical small challenge now is to compute, for each layer section, both the radius and the extension of the arc of the circular section around which it must be swept, to generate the right profile on the straight side. ext_int_dent

The only references I had were the radius of the inner part of the more external dent (in green here besides) and the length of the straight side. As the frame should be square-like, starting from the side length (l), with the inner radius (r), it’s easy to compute the arc of circumference needed to have the same length (360*l/2πr) on the curved side. I drew the sketch on the x-z plane at the proper distance from the revolution (x) axis. The more external layer is then quite straightforward, as in the picture below, superimposed on the section sketch.


ext_lay_revRevolving it around the x asis for an arc of the above computed amplitude, creates the more external layer.

The intermediate layer layer must be created in two steps: a thicker layer longer layer from which a shorter thinner layer (corresponding to the right side lower dent in the picture) must be cut out (the right side of all the layers coincide with the middle point of the straight side).


To create the same indented profile altwo_layong the straight side, this layer must be swept along an angular amplitude which is less than the external one of an amount corresponding to a circumference part as long as the dent, using the same formula as above to extract the arc difference (arc_diff = arc_complete * dent_l/side_l).

Now it’s time do draw and revolve the innermost layer to cut out the internal dent from the just created layer (as the others, matching the same side length at the right side of the sketch, out of the picture).


Again, the sweep arc is shorter w.r.t. the previous, of a distance matching on the circumference, the horizontal distance in the two dents. In the picture here below the internal layer is show as wireframe, while the thin coloured layer is the newly generated to be cutout from the previous.


The quarter of the frame is now ready with the proper shape:


It needs only to be cut through in the middle: again, a sector of cylinder with the arc amplitude matching the horizontal upper extension of the section sketch does the job: here below the quarter of the frame and the detail of the straight side section: the profile of the original section sketch, just “curved” to match the cylinder shape.

Even if this solution required more time and some geometrical computations, I’m more satisfied of it’s elegance, w.r.t the previous one. The final result, of course, is the same.

A curved frame: solution one

I’ve been asked to design a rectangular frame with a geofr_sectmetric profile.

It seems to be child’s play for any parametric 3D CAD designer, but…frame

…the frame must be plugged in a rectangular widow cut out from a pipe: it must be bent around a cylindric surface…


…so the section of the frame along the straight side must be curved.

Using FreeCAD, as usual, it is indeed child’s play to draw the sketch of the section of the frame, as well as to sweep it either along the arc of circumference or along a straight segment, but… the section of the frame along the straight side must be curved to match exactly the curvature of the arched side with the above geometric (not curved) section and to follow the pipe’s shape.

Taking into account the symmetry of the final frame, it is enough to design a quarter of it, with the curved and the straight half sides matching at the corner.

As first attempt I draw the cylinder sector corresponding to the frame, then I extract the curved surface with the Face Binder tool and I extract the outer perimeter of the surface: it is the path along which the frame will be built.

I position the sketch of the section with the proper orientation, exactly at one vertex and I sweep it along the curved side of the path.

The generated curved side of the frame must be cut at 45° w.r.t. the section plane, to match it with the linear side to be designed:on the sketch of the frame section I draw a rectangle, bigger than the section shape and sharing it’s external edge, I revolve it around the shared edge for 45 degrees inwards to the frame: the generated  wedge can be used as cut tool to chamfer the rectangular ended curved frame side.

The new 45 deg sloping end face can be extracted (again with the Face Binder tool) and swept along the straight side of the path. sloping_faceThe generated half straight side will perfectly match the curved side at the corner, but will end with a 45° sloping face, which will completely intersect and overlap with the corresponding ending in its mirrored copy.

The first prototype, ready before the deadline was fine. I was nevertheless not yet satisfied of this solution: working fine but not elegant from a design point of view. In the next post, the next design solution.