I love designing in Siemens NX, but keeping these files on my hard drive doesn't help anyone. I decided to put them out here for anyone who needs to practice material. Whether you're a student or just love CAD like I do, feel free to use these blueprints to sharpen your skills.
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Shaft End Support Block
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CAD Modelling Challenge #8 — Engineering Drawing Breakdown
NX Modelling Challenge #8 | NXDATUM 04DTM23
This week's challenge features a classic Clevis Joint or Yoke. This component is a staple in mechanical engineering linkages, actuators, and pneumatic cylinders. It is an excellent exercise because it combines both turned (cylindrical) features and milled (prismatic/forked) geometry into a single solid body. Paying close attention to the origin planes for your dimensions is critical here.
The Stepped Shaft (Rear Section)
Starting at the back, the model features a stepped cylindrical shaft. The total length of this protruding section is 80mm, measured from the back face of the main rectangular block.
The primary shaft has a diameter of Ø25 and a length of 55mm, ending with a precise 3x45° chamfer. The larger mounting shoulder has a diameter of Ø40, which covers the remaining 25mm of the shaft's length (80mm total - 55mm step).
The Main Body & Clevis Fork (Front Section)
The main body begins with a solid rectangular base that is 52mm wide, 60mm high, and 15mm thick. From this base, the two arms of the clevis extend forward.
The overall width remains 52mm, but an internal pocket is cut out to create a 32mm wide gap, leaving two parallel arms that are exactly 10mm thick each (10 + 32 + 10 = 52). The arms extend forward from the block, terminating with a full R30 radius that perfectly matches the 60mm overall height.
Hole Placement & Constraint Logic
There are four through-holes in total across the two arms, labeled as 4-Ø10. Their vertical placement is exactly centered at 30mm from the bottom edge.
For the horizontal placement, trace the extension lines carefully: they originate from the back face of the main block. The first hole is centered at 62mm from the back face, and the second is at 94mm from the back face. The distance between the two hole centers is explicitly given as 32mm (94 - 62 = 32), which serves as a great dimensional check.
Modelling Strategy in Siemens NX
For a clean and robust feature tree in Siemens NX, try this sequence:
Base Extrusion: First, sketch the side profile of the main block and the solid fork (including the R30 end profile and the 60mm height) on a primary datum plane. Extrude this symmetrically to the total width of 52mm.
Internal Cut: Next, create a sketch on the top face to draw the 32mm wide rectangular inner gap, and use Extrude (Subtract) to cut it out, stopping exactly at the 15mm thick base wall.
Rear Shaft: For the rear shaft, sketch the two concentric circles (Ø40 and Ø25) on the back face and extrude them to their respective 25mm and 55mm lengths.
Final Details: Finally, use the Hole command for the four Ø10 holes and apply the Chamfer feature to the front of the shaft.
What This Challenge Tests
This model evaluates your ability to combine features that would traditionally be machined on different equipment (lathe vs. milling machine). More importantly, it tests your blueprint reading skills—specifically your ability to trace dimension lines back to their correct origin face rather than assuming they start at the nearest visual edge.
Complete the model in Siemens NX, run mass properties, and submit your answer on the NXDATUM validation tool.
Created by NXDATUM | Siemens NX CAD Modelling Series | All dimensions in mm | Scale 1:1
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