Design of Machining.pptx PPT FOR DESIGN X

PPT FOR DESIGN

1. Design of Machining Design features to facilitate machining UNIT III

2. Key principles Minimize setups: design with symmetry, datum faces and features that let the part be machined in a single clamping when possible. Use standard sizes: standard drill sizes, stock, threads and feature spacing speed work and reduce cost. Design for fixturing: add flat faces, pads, bosses or datum features where clamps and vises can grip. Specify realistic tolerances & finishes: tighter tolerances raise cost — only call them out where necessary. Make cutting simple: avoid tiny radii, deep narrow slots, and awkward internal corners that require special tooling.

3. Useful design features & guidelines 1. Corners, fillets & radii Use fillets on internal corners — internal fillet ≥ cutter radius . If you expect a 6 mm endmill, use fillets ≥ 3 mm. Avoid sharp internal 90° corners (require EDM or small cutters). External corner radii: 0.5–1 mm is usually fine for hand work; larger radii improve tool life.

4. 2. Hole design Prefer standard drill sizes (or metric +0.1 mm clearance holes for bolts). Edge distance: keep hole centers ≥ 2× hole diameter from edges (better: 2.5× for critical parts). Depth-to-diameter for drilling: keep ≤ 3:1 when possible (e.g., for a 10 mm hole do not exceed ~30 mm depth) to avoid wandering and need for special long drills. For threaded holes, use standard thread depths (e.g., M6 × 1 thread depth ~1.5× nominal diameter for blind holes).

5. 3. Wall thickness and pockets Keep walls stout — thin walls vibrate and deflect. For machined aluminum , avoid < 1.5–2 mm unsupported walls; for steel, slightly thinner is acceptable but still avoid <1 mm. Pocket aspect ratio : shallow and wide > deep and narrow; deep pockets require long tools and slow feeds. If deep pockets are needed, add access slots or design to allow roughing then finishing with shorter tools.

6. 4. Slots and keyways Make slot widths match standard endmill sizes (e.g., 3, 4, 6, 8 mm) so a single pass can create them. Keep slot depth ≤ 3× width where possible . 5. Threads and tapped holes Use thread inserts ( Helicoil ) for soft materials or repeated assembly cycles. For through-bolts prefer clearance holes rather than tapped holes when possible (easier and faster).

7. 6. Chamfers vs. radii Chamfers are easier to cut than internal radii in many contexts and are helpful for assembly. Typical chamfer: 0.5–1.5 mm at 45 ° . 7. Datum and locating features Provide at least three orthogonal datum faces (flat surfaces, bosses, flats on round parts) to permit repeatable fixturing. Add registration flats on round parts so they locate in a vise or jig.

8. 8. Symmetry & orientation Make parts symmetric about machining planes to reduce the number of re-setups. Orient critical surfaces to be machined from the same setup when possible . 9. Stock allowance & finishing Leave a small machining allowance for roughing: 0.5–1.0 mm for finishing faces (depends on process/material). If using near-net shapes (castings, forgings), indicate final machine allowances on the drawing.

9. 10. Surface finish & tolerances Default practical tolerances: ±0.1 mm for general features; ±0.02–0.05 mm for precision fits — call out only where needed. Surface finish: list Ra only for surfaces that require it; tighter Ra increases cost . 11. Tool access & cutters Ensure straight-line tool access for endmills and drills; avoid undercuts unless you plan for special tooling or EDM. Design around common tool diameters — smaller cutters are slower and more fragile.

10. . 12. Minimizing special operations Avoid features that need EDM, deep small-diameter holes, internal threads in blind deep holes, or complex 3D curves unless essential.

11. Material & process considerations Aluminum : forgiving, use larger corner radii, avoid very thin webs. Steel : slower feeds, but thin walls slightly more feasible. Plastics : watch for melt/deflection; use shallow engagement and plenty of support. Tell your machinist the material early — it affects recommended feeds, speeds and tooling.

12. Quick design checklist Are critical surfaces on one setup? Y/N Are fillets ≥ cutter radius where practical? Y/N Are holes standard sizes and ≥ 2×D from edges? Y/N Is depth:diameter ≤ 3:1 for drilled holes? Y/N Are wall thicknesses ≥ 1.5–2 mm (aluminum) or ≥1 mm (steel)? Y/N Are slots made to standard endmill widths? Y/N Are tolerances as loose as practical (default ±0.1 mm)? Y/N Is there a flat or boss for fixturing? Y/N Avoided undercuts/EDM unless necessary? Y/N