Datum B Is a Slot: Drawing and Model Disagree
A 1.2 mm thick 301 stainless half-hard bracket is to be blanked and formed in a compound die. The customer drawing shows six Ø4.00 +0.05/0 holes with a feature control frame: position Ø0.15 Ⓜ to datum A (the flat face), B (a 20.00 +0.10/0 wide slot), C (the left edge). Basic dimensions locate the holes from the slot centreline and from datum C. The slot is also the locating feature in the customer's weld fixture. Notes require breaking all sharp edges 0.2-0.4 mm and call 0.8 µm Ra on a formed inside radius of 0.6 mm in 1.2 mm material. The customer's STEP model places the holes 0.20 mm from the basic dimensions on the drawing. The die is due in five working days and the customer's buyer is pressing for release.
1. Explain how the datum reference frame should be established for layout and inspection, and why datum B being a slot changes how you build the die.
Read the worked answer
A is the primary datum: the flat face contacts three points and orients the part. B is a 20 mm slot, which constrains two degrees - translation across the slot and rotation about A - provided the datum is taken at the slot centre. C is the tertiary edge, one point. The frame is therefore A (3), B (2), C (1).
Because B is a slot and is also the weld-fixture locator, hole position relative to the slot centreline is what matters functionally. If the slot width varies from 20.00 to 20.10 and the part is located on one side, the effective centreline shifts by half the width variation. Build the die to locate on a plug or expanding mandrel at the slot, confirm with the customer whether datum B is the slot centre plane or one side, and design the strip layout so the slot and holes are produced in the same station to avoid stack-up.
2. Identify the requirements that conflict or cannot be met as stated, and describe the formal action you take before cutting steel.
Read the worked answer
Conflicts to raise:
- 0.8 µm Ra on a 0.6 mm inside radius in 1.2 mm half-hard 301 is not realistically producible or inspectable; a standard stylus cannot access the radius cleanly, and the material will spring back and may crack at that radius.
- The edge-break note 0.2-0.4 conflicts with the natural burr side of a blanked part; it must state which edges and which side.
- The STEP model is 0.20 mm from the drawing basics. Drawing dimensions govern unless the customer states the model is basic, so do not split the difference.
- The Ⓜ modifier combined with a slot datum needs written clarification of the datum feature simulator.
Action: raise a formal RFI or deviation request with a marked-up drawing, hold layout release, and get written disposition before cutting steel. Notify the buyer in writing that the five-day date is at risk because of the drawing query, not the shop.
3. Explain how the Ⓜ modifier affects punch sizing and how you would inspect the holes functionally.
Read the worked answer
Ⓜ means the Ø0.15 tolerance applies at MMC of the hole (Ø4.00). As the hole departs from MMC, the allowable position error grows by the same amount: at Ø4.05 the total is Ø0.20. This is bonus tolerance and it is real, not a paperwork nicety - it reflects the functional clearance in the weld fixture.
Punch sizing: the punch produces the hole, so make the punch near the high limit, about Ø4.04-4.05, so wear drives the hole toward the low limit rather than below it. Die opening = punch + 2 x clearance; for 1.2 mm 301 half hard, allow roughly 5-7% per side, about 0.07-0.08 mm.
Inspection: build a functional gauge with pins at virtual condition Ø4.00 - 0.15 = Ø3.85 at the basic locations. A part that accepts the gauge is good. Use CMM with bonus evaluation for process control, but treat the gauge as the referee in a dispute.