First
things
first.

Let's start
with the easyest part

A holed cylinder, with a cylinder at the top, sketch of circunferences and boss-extrude

From the list of components, I proceeded to an ordering by 'suspicious' of difficulty in modeling, starting the process with the component that seemed to be easier and faster to execute.

The eccentric cylinder that allows the transmission of rotational movement to lateral movement was chosen. Don't forget to get the caliper… you're always on my side.

The process:
  1. Selection of top plan (by default I always start with this plan. Will there be an advantage in another one?. Is any other criterion useful at this time, which will eventually optimize the future assembly process?)
  2. Open sketch and define a circunference from the center. Smart Dimensions and insertion fo the desired diameter.
  3. Boss-estrude… dimension in one direction, commit and we have the first cylinder… Still missing the hole. New Sketch at cylinder base normal, centered circumference, diameter, cut-extrude, depth, commit
  4. Second cylinder: select normal to the top of the first cylinder, and repeat the process: skecth, circumference (this time defined by 3 points, one of them being tangent to the top circumference of the first cylinder); smart-dimension for diameter; boss-extrude.
  5. Detail… small fillet at the end of the smallest cylinder How? Feature fillet, face selection, symmetrical, 0.25mm.

The engine
is just a block

... or 3 bodies

For this exercise I will consider the engine as just a motionless volume. Again the same strategy…, skecth and vertical boss-extrude.

The process:
  1. Top plan selection
  2. For this process, I adopted a composite drawing strategy for the basic boss-extrude sketch. A rectangle and a concentric circunference. With the Trim to Closest option, from the Trim Entities tool, I removed the superfluous lines.
  3. Boss-estrude... dimension in one direction, commit and we have the engine body.
  4. Then two more stacked cylinders, by sketching the normal top of the previous cylinder and their boss-extrude.

One step forward,

... but keeping it planar

In the modulation of this piece I encountered some of the first challenges ..
1 + 1 is not always equal to 2 ..
and the problem of overdefining dimensions.

In this process I adopted the line-by-line drawing, defining each dimension .. but due to inaccuracies in the dimensional survey with the caliper, the sum of the parts, at first, did not fulfill the dimension of the whole.

Commitments have been made .. adjustments will be made later at assembly time.

The process

PPART 1 - Create the flat part of the part
  1. Top and sketch plane selection.
  2. For this process, I adopted a line-by-line drawing strategy. For each segment, I sequentially carried out the dimensional survey of each one.
  3. When closing the perimeter, symmetry was not achieved and the sum of the parts was greater than the whole. I discovered the possibility of duplicating and inverting. No more. Erase and redo...
  4. Lines the line, but only half the shape, starting from a midpoint.
  5. Define and position the 2 holes (rectangles) in the upper half of the shape already defined. I discovered the possibility of positioning the rectangles within the shape's perimeter, using the dimensions tool. After all, it also serves to define distances.
  6. Let's see then how to duplicate and invert 180°... Mirror entities.. define a midline hinge (Yes.. lines can be construction lines) and mirror.
  7. Oops... some corners are curved... solved with Sketch Tools > Fillet.
  8. Another unique rectangle and 1.5mm boss-extrude

PART 2 - Raise a hollow cylinder on one side
  1. I selected the normal of the top plane of the already defined plate.
  2. Create a sketch to define a circle tangent to the shape's sideline.
  3. Expand (Offset Entities) so that the volume wall comes out 0.75m outside the plate.
  4. 5.5mm boss-extrude to heighten the volume.
  5. To empty the interior of the volume, I used the Shell tool, on the base face of the same, with a 0.75mm wall (the same dimension previously defined in the offset
  6. Problem!! The base of the plate keeps the set closed, hiding the leak created. Solution: Open a new orifice, coinciding with the inner circumference created by the Shell, on the initial plate (Part 1)
  7. I went back to the Plate Sketch, defined a new circumference tangent to the shape... Commit... and updating the shape revealed the new circular opening, revealing the interior of the cylindrical volume.

And now for something completely different.

Multiple planes, .. and some angular ones!!

In addition to the previous strategies, using sketches and boss-extrudes, this piece brought the challenge of modeling parts from different planes, out of phase and with different angles.

The process

PART 1 - The first body and the creation of a new vertical-lateral plane
  1. Top and sketch plane selection.
  2. The line strategy was used to design the base of this piece in a trapezoid shape with the respective openings, resulting in a flat first body, 0.6mm thick.
  3. Next I tried to draw the vertical walls at the ends of the 'antennas' attached to the base body.
  4. Define a new vertical plane, as the base of the new sketch, using 3 reference points. As the body already drawn, only provided me with 2 reference points, I resorted to drawing a construction line along one of the points, using one of its points as a third reference for the new plane.
  5. With the plane defined, I created a new sketch, in which I defined line by line, the polygon to which a 1mm Boss-extrude would affect.

PART 2 - The second volume and how to create an angular plane
  1. The idea would be to project the walls in a new way in front of the piece, in a direction 45º from the top face of the already defined flat body.
  2. After some research, I opted for the initial creation/definition of a hinge line (Reference Geometry > Axis) defined by the front and top faces of the already defined body.
  3. Then the definition of the desired plane (Reference Geometry > Plane) through the indication of the created hinge and the top face of the body already defined, and replacing the default parameter Coincident, by an angle of 135º.
  4. With the angle defined, I selected its normal one, and proceeded in a similar way to the definition of the previous shapes, through sketches and boss-extrude.
  5. This volume resulted in 2 bodies, in which I left the Merge result option disabled for one of them, due to a construction error. I suspect it may be related to the overlapping of the 2 bodies, but it lacks more dedicated verification.

PART 3 - Finishing the first volume
  1. With the biggest challenge of this piece solved, I went back to finishing the initial form, defining the end of the other 'antenna' in the same way as mentioned for the first one.
  2. Finally, I opened a new sketch for the definition of the 2 circles, which allowed to extrude the hollow cylinder in one of the ends.
  3. In this sketch I defined a construction line in the middle of the shape, which allowed me to mirror entities from the cylinder to the other end of the part.

Time for a break.. let's make some drawings

To much automatic.. should try again later with more control

Given the greater geometric complexity of the last piece, I chose this one to create the first technical drawing. At this point, I only used the automatic creation provided by Solid Works. I made a first and brief recognition of the options presented, feeling the need for greater exploration and control over the result.

I did however configure the rendering method for the first quadrant, via the Solid Works properties menu.