• The three bend allowance tables in the Machinery's Handbook (Industrial Press) are based on three different formulas which use a constant fraction K for each different material.
• For soft materials such as soft copper and soft brass, K is always .350.
• For medium-hard materials such as soft steel, K is always .408.
• For hard materials such as bronze, CRS, and spring steel, K is always .452.
• The fact that these tables do not recognize variations in K (as the radius and the thickness change) makes them unacceptably inaccurate. The use of a different K for different radius bends (determined by the first formula above) yields much more accurate results.

Even when using the more accurate fraction K from the first formula above, we must keep in mind that any formula based on experience is still only a theoretical approximation. In the case of sheet metal bends, the above formulas do not take into account several facts.

• The thickness of the material changes slightly at the bend.
• The center of the neutral arc is not exactly coincident with the center of the inside radius.
• Material deformation (stretching and compressing) is not entirely limited to the theoretical boundaries of the bend.
• The neutral plane does not form a perfect cylinder, but "bells out" at its edges (this effects bends in very narrow strips more than wide strips).
• The fact that these tables do not recognize variations in K (as the radius and the thickness change) makes them unacceptably inaccurate. The use of a different K for different radius bends (determined by the first formula above) yields much more accurate results.

Even so, the error introduced by these factors is far less than the error introduced by the assumption of a constant K.

However, there are many production factors which can affect the actual amount of material used in a given bend.

• True material thickness may vary from the specification.
• Certain production methods will stretch the material more than others.
• Forming tools may not bottom completely, producing inaccurate bends.
• Multiple bends done in one operation may trap panels and thus increase elongation.
• Temperature and direction of grain affect the bend allowance.

Since the designer usually cannot control these factors, he/she must offer the best general estimate possible and expect those who fabricate the part to know how to compensate for these factors as needed. See the following articles:

Hole Sizes

Holes are produced by mechanically pressing a punch tool through the sheet metal in order to rip out a slug. When the punch retracts the slug remains stuck in the die tool and a hole is left in the sheet metal. The size and shape of the punch and die tooling govern the size and shape of the hole produced in the sheet metal. For strength, the punch tip must usually be at least as large as the sheet metal thickness.

The die tool must be slightly larger than the punch to minimize tooling wear and to reduce the pressure required to punch the hole. The die clearance is generally about 10% of the material thickness. For example, the material is .100 aluminum and the punch diameter is 1.000", the die diameter would be 1.010". The size of the hole on the punch side will be the same size as the punch tool. The size of the hole on the die side will be the same size as the die tool.

Except for tooling wear, there is very little variation from one hole to the next. SMI has an extensive library of tooling, but we do not stock all possible tool sizes. We look to the engineers and draftsmen to give us a tolerance range that allows us to use our existing tooling. When that is not possible, a capital investment in new tooling is required. Generally speaking, +/-.003" (.08mm) is a reasonable hole size tolerance. Keep in mind, however, that we are measuring what will pass through the hole, not the "rim sizes" of the hole.

Hole to Hole

The accuracy of the distance from one hole to another hole is largely dependent upon the machinery. SMI's equipment will hold better than +/-.005" (.13mm) with little difficulty. However, each hole that is punched introduces stress into the sheet metal. If the part has many holes closely spaced, like a perforated pattern area, the result can resemble a baker rolling cookie dough -- the sheet metal can be expanded causing unwanted variation between holes. If this condition exists, a greater tolerance should be applied to certain areas surrounding this characteristic

Hole to Edge

Because the profile (or edges) of the part are generally punched just like any hole, the same considerations for hole-to-hole apply. When punching very near to an edge (less than 2X material thickness) the edge will be pushed out by the stress of punching the metal. This edge migration introduces variables in the accuracy of the hole location. Whenever possible, engineers should allow +/-.010" (.25mm) hole-to-edge. Resort to +/-.005 (.13mm) only when absolutely necessary.

Hole to Fold

There are several variables introduced leading up to this stage in the fabrication process. The part has been punched on a CNC Turret Press, sanded or tumbled to remove burrs, and is now being bent on a Press Brake. The deburring process may remove .003" (.08mm) when cosmetic appearance is a priority. Precision Press Brakes will position and repeat in less than .001" (.025mm). Well trained and skilled operators will be able to load the parts for forming consistently from bend to bend. Nevertheless, engineers must consider the natural variation in material thickness (5% of nominal thickness), the +/-.005" (.13mm) from the turret press, the effects of cosmetic graining, and the variation introduced by the press brake. Whenever possible, engineers should allow +/-.015" (.38mm) hole-to-fold. Resort to +/-.010 (.25mm) only when absolutely necessary.

Fold to Fold

All of the considerations of "hole to fold" apply, compounded by the fact that multiple material surfaces and thicknesses are involved. Whenever possible, engineers should allow +/-.020" (.50mm) fold-to-fold. Resort to +/-.010 (.25mm) only when absolutely necessary.

Best Practice in Tolerance Specification Although the machinery and tooling will repeat within .004" (.10mm), it is a mistake to simply engineer all mating parts expecting +/-.005" (.13mm) accuracy. Such over kill forces additional labor in sorting and inspection. The result of tolerances that are too tight is simply higher cost and lower productivity. Correctly toleranced parts still have excellent fit and function, with the added benefit of efficiency.