How to make a sheet metal technical drawing.

One part. Two different drawing jobs.

Use the formed drawing to accept the finished part. Use the flat drawing to communicate the developed blank.

This worked example uses a real three-bend bracket in Onshape and Xeon NC’s website entry for 0.100″ 5052-H32 aluminum. Its broad top flange, long side web, lower mounting ear, and small slotted flange show why one overall dimension is not enough.

Dimension surfaces you can actually check.

For this example, assume the broad top flange is the assembly’s seating face. Start the inspection scheme there. Confirm that assumption against the mating assembly before establishing formal datums.

Finish the location scheme.

A practical datum scheme could use the main seating face as A, a perpendicular locating face as B, and a suitable end face or locating feature as C. Choose these from how the bracket is constrained in its assembly, not from whichever edges are easiest to click.

Locate the round mounting hole in two directions and give its diameter. Give the slot’s width, overall length, orientation, and center location. If the slot provides adjustment, protect the direction that controls alignment and allow the intended travel in the other direction. Include the required formed offsets between these features; a perfect flat hole pattern can still miss its mating part after bending.

Use section or detail views where offsets, internal clearances, or short bend tangents are hard to see. Add appropriate position, orientation, or profile controls when ordinary size dimensions do not express the function. Thin sheet may need an agreed restrained inspection condition; never clamp a part into compliance without specifying that condition.

Call out the inside arc: R0.126″.

The radius dimension belongs on the inside cylindrical bend surface. Use the Onshape radial dimension tool on the inside arc in a view normal to the bend axis, or add a section/detail view that exposes it clearly. Keep the leader on that arc and leave room for the value.

For this example, the nominal inside radius is 0.126″ and the stock thickness is 0.100″. The ideal geometric outside radius is therefore 0.226″ = 0.126″ + 0.100″. The outside radius is useful for explanation or clearance calculations; it should not become a second independent acceptance requirement unless the design needs it.

All three bends currently use R0.126″. A common note can cover identical bends, with exceptions called out individually. Specify the radius tolerance required by the design and accepted by the shop; a three-decimal display alone does not establish that tolerance.

How to inspect the radius

A radius gauge gives a quick comparison when there is enough accessible arc. Use an optical profile measurement, CMM, or agreed contour method when the radius is critical. Inspect away from distorted reliefs and cut edges. Measuring two straight faces with calipers does not independently verify the bend radius.

Match the material row, not a generic K-factor.

The current Xeon bending data identifies the following setup for 0.100″ 5052-H32. The tool identities can be checked in the press-brake tooling library.

The punch’s R1 marking is not the finished R0.126″. R1 is a 1 mm tool-tip radius; the air-bent part’s resulting radius depends on the die opening, material, thickness, and process. Likewise, the die’s R2 marking is not a 2 mm finished inside bend specification.

The 20 mm opening is about 7.87 times this stock thickness. It fits the tooling library’s screening guidance, but the small slotted flange still needs adequate die support. Check reliefs, slot-to-bend distance, tooling clearance, bend sequence, and tonnage. A 1.000″ outside flange height by itself does not prove every contact or collision check passes.

Check every bend, including overrides.

The original model had R0.125″ and K = 0.45 defaults, plus a Modify joint feature that repeated those values as overrides. Updating only the default would have left that joint inconsistent. The example now uses the model radius and K-factor for that joint, and its bend table reports all three bends at R0.126″ with approximately 0.261″ bend allowance.

Calculate the bend once. Do not compensate twice.

For an ordinary circular bend, let θ be the bend rotation from flat, in radians; R the inside radius; t the thickness; and K the neutral-axis factor. At a 90° bend, θ = π/2.

That calculated bend deduction rounds to Xeon’s listed 0.1912″. Onshape’s table displays the allowance as 0.261″ because of its display precision. Keep full precision in the model and round only for presentation.

For example, two hypothetical 2.000″ outside legs with this single 90° bend develop to 4.000 − 0.191248 = 3.808752″. Those are demonstration leg lengths, not dimensions taken from this bracket.

This bracket branches into separate flanges. Trace each development path through the bends it actually crosses. Do not subtract three bend deductions from the bounding-box length just because there are three bends. Let the validated sheet metal model develop the complete outline, then independently check representative paths.

When the CAD flat pattern already uses the approved allowance or deduction, do not apply the same compensation again in the cutting file or CAM system. Choose one owner for the production development.

Validate against an actual bend when needed.

Use a test coupon of the same grade, temper, thickness, tooling, and bend process. Measure the actual thickness, final angle, radius, and leg lengths. For a 90° coupon measured to outside virtual-sharp intersections, BD = outside leg 1 + outside leg 2 − known blank length. Compare that result with the table and adjust the controlled bend data with the shop if needed. Angle correction alone cannot recover an incorrectly developed blank length.

Show the blank and the bend instructions.

Create this view in Onshape by right-clicking the Part Studio’s flat pattern and choosing Create Drawing of Flat pattern of Part 1, or insert its flat pattern in an existing drawing. Use a readable scale and check every generated bend note against the formed model.

• Identify the viewing side. All three current notes say DOWN 90° R.126, relative to the shown flat view. UP/DOWN is not an absolute shop-floor direction.
• Locate bends unambiguously. Show bend centerlines and a bend table or clear notes. Add locations needed by the agreed manufacturing workflow; separate cutting geometry from bend-line geometry in the DXF as the shop requires.
• Define the rest of the blank. Overall length and width do not define the reliefs, corner radii, hole, or slot. Supply the controlled profile file and the remaining drawing requirements.
• Keep notes readable. Move crowded notes or use a bend table at release. Default placement on bend lines is useful while developing the drawing, but it can obscure a dense profile.
• State responsibility. If Xeon develops the production blank, mark the supplied flat pattern as reference under that agreed workflow. If it controls cutting, identify its revision and approved bend-development data.

Release the folded model, drawing PDF, and any flat DXF together at the same revision. Confirm both the cutting geometry and the finished inspection requirements before manufacturing.