Orthographic views, dimensioning, CAD sequence and manufacturing for a twin-tower saddle bracket: 04-BS-15, Undated paper, Q1

Question 1: Orthographic views, dimensioning, CAD sequence and manufacturing for a twin-tower saddle bracket (50 marks)

Question text not reproduced: the examination questions are © Engineers and Geoscientists BC. Open the official past paper (linked at the top of this page) to read the question, then follow the worked solution below.

[Figure not reproduced: Given isometric pictorial of the twin-tower saddle bracket. See the official exam paper or the cited reference text.]

Fig. Q1 — given isometric pictorial: a base slab with a 45° wedge ramp at the front-left, a twin-tower block with a concave semicircular saddle cut between the towers, two through-holes in the exposed base shelf, and a stepped/rounded right-hand end.

Given. A cast/machined bracket comprising: a flat base slab; a front-left wedge ramp rising from the base to the top of the taller (left) tower; a taller left tower and a shorter right tower separated by a concave semicircular saddle spanning the full depth; a rounded step-down at the far right returning to base height; and two vertical through-holes drilled in the base shelf in front of the towers. Check: the pictorial gives no printed dimensions (per Note 1, use “xx”) and the saddle/fillet curvature must be read from the freehand sketch; the proportions used below are the single self-consistent solid that reproduces every visible edge, face count, and hole position in the given pictorial — a competent candidate's sketch need only be topologically equivalent, not pixel-identical.

a) Orthographic views (third-angle projection)

Approach. Orient the part with the base resting on the horizontal projection plane and the wedge ramp facing the viewer; project the Front, Top and Right-side views using the third-angle glass-box arrangement (Top view above the Front view; Right-side view to the right of the Front view, all aligned on shared projectors). The saddle cut and the two holes are read directly off the pictorial; the rounded right-hand step and the ramp both project as straight fold-lines in the Front view and as visible lines in the Top view (their curvature belongs to the physical fillet radius, not to the sketched proportions).

Fig. Q1a — Front, Top and Right-side views in third-angle projection. Dashed lines = hidden detail (the two base holes in the Front view; the saddle-depth and notch boundaries in the Right-side view).

The wedge ramp appears as a sloped straight edge only in the Front view (it is a planar chamfer, constant through the full depth, so the Top and Right-side outlines stay rectangular there); the saddle appears as a genuine curve only in the Front view, and as two straight fold-lines (its front and back edges) in the Top view, since the cut runs parallel to the line of sight in that view.

b) Dimensioned sketch

Approach. Add one complete, non-redundant set of size and location dimensions per view following ASME Y14.5 practice: overall size dimensions on the outermost extension lines, feature-location dimensions referenced from a common datum edge (the base's front-left corner), and a diameter callout with the "2X" multiple-feature prefix for the two identical holes — every numerical value replaced with "xx" per Note 1.

Fig. Q1b — dimensioned views: overall length/width/height, hole spacing and diameter (2X DIA xx), all referenced from the front-left datum corner. Values withheld per the exam's own instruction ("xx" in place of numbers).

Dimensioning rules applied: dimensions placed on the view that shows the feature's true shape (the hole diameters are called out on the Top view, where the holes read as true circles, not on the Front/Side views where they are hidden width-lines); no dimension is duplicated between views; overall envelope dimensions are placed outside feature dimensions so extension lines never cross witness lines.

c) Feature-based solid modelling sequence

A parametric, feature-based CAD package (e.g. SolidWorks, Inventor, Fusion 360) builds this part as an ordered tree of parametric features, each referencing a 2-D sketch on a plane or face:

Base extrude. Sketch the base slab's rectangular profile on the Front (XZ) datum plane; extrude it (Boss/Base Extrude) through the full depth to create the solid base.
Tower extrude. Sketch the twin-tower footprint (full width, full depth) on the base's top face; extrude upward to the taller tower height, forming one continuous raised block spanning both towers.
Saddle cut. Sketch a semicircular profile on the tower's front face, centred between the two towers; use an Extruded Cut (through-all, in the depth direction) to remove the saddle material, leaving the two towers standing.
Wedge-ramp chamfer. Sketch the ramp's triangular profile on the left end face; Extruded Cut through the full depth to create the sloped front-left ramp (a simple linear chamfer feature could also be used if the ramp angle is constant).
Right-end fillet/step. Apply a Fillet feature (constant radius) to round the top-right corner down to the base surface, or, if the step is flat-faced, an additional Extruded Cut.
Hole feature. Use the Hole Wizard (or a sketched circle + Extruded Cut, through-all) to place the two identical through-holes on the exposed base shelf; the Hole Wizard is preferred because it auto-updates if the plate thickness changes and it tags the holes for a hole-callout in the drawing.
Pattern (optional). Since the two holes are identical and evenly spaced, a Linear Pattern from a single hole feature (rather than sketching both independently) keeps the design intent explicit and lets the spacing be edited from one dimension.

This feature order (base → tower → saddle cut → ramp cut → fillet → holes) mirrors the actual manufacturing sequence — roughing the block, then machining the details — which is good parametric-modelling practice: it keeps the history tree stable, since later cosmetic features (holes, fillets) reference the already-finished bulk shape rather than the other way around.

d) Manufacturing methods and issues

The part's rectilinear towers, planar ramp and simple through-holes are all achievable on a 3-axis vertical milling machine: rough the block from bar/plate stock, face-mill the top surfaces, then machine the saddle with a ball-nose or radiused end mill sweeping the full depth, cut the ramp with the head tilted to the ramp angle (or with a dovetail/angle cutter), and drill (then ream, if a precision fit is required) the two holes on a single set-up using the base as the locating datum. For higher volumes, the bracket is a good candidate for sand or investment casting near-net-shape followed by a light finish-mill pass on the mating faces and holes, which reduces machining time at the cost of tooling (pattern/die) investment.

Issues to anticipate: the concave saddle needs a cutter radius no larger than the saddle's own radius, or the tool will gouge the adjacent tower faces — the CAM programmer must check tool-radius clearance before posting the toolpath. The two holes, drilled through a shelf that is thin relative to the tower height, are prone to drill wander/breakout unless spotted first with a centre drill. The sharp internal corner where the saddle meets each tower's vertical wall is a stress concentration in service and should carry a small fillet (not a sharp re-entrant corner) both for tool life during roughing and for the finished part's fatigue life. Finally, the asymmetric mass distribution (tall left tower vs. short right tower) means work-holding must clamp low, on the base, so cutting forces do not tip or chatter the part.

Topic: Third-angle orthographic projection, engineering dimensioning, and feature-based parametric solid modelling.

Key relations: Third-angle glass-box rule (Top above Front, Right-side to the right of Front, all views aligned on common projectors); ASME Y14.5 dimensioning (true-shape view carries the size dimension; datum-referenced location dimensioning; "2X" multiple-instance prefix); parametric feature tree = ordered sketch-based operations (extrude/cut/fillet/pattern), each referencing prior geometry.

Why this works: Three mutually-perpendicular orthographic views, taken together, fully define a solid's geometry without ambiguity (each view resolves the depth axis the other two collapse); a feature tree that follows the physical roughing-then-detailing sequence stays robust under later design changes, because downstream features depend on the already-resolved bulk shape.

Common pitfall: placing a hole's diameter dimension on a view where the hole shows as a hidden line instead of the view where it reads as a true circle; building fine details (fillets, holes) before the bulk shape in the feature tree, which makes the history fragile to edit.

Source: Bertoline & Wiebe, Technical Graphics Communication, ch. on multiview projection and dimensioning practice; Giesecke, Technical Drawing / Engineering Graphics, ch. on solid modelling and manufacturing processes.