Practical Sheet Metal Design Part 2

Practical Sheet Metal Design Part 2

Tolerances for Sheet Metal parts:

A bit of history first: When I started working in sheet metal in 1975 we generally worked to +/- .063 inches. In the shop I worked at initially there wasn’t a pair of calipers to be found. Everything was checked with a tape measure. When I interviewed at Byers Precision it was stressed to me that they worked to much closer tolerances, .010 - .015 typically. This led to a funny story…On my first day on the job I was given a print, told to figure the flat pattern, shear, punch & form the part. With the interview still fresh in my mind I determined to accomplish making this part to the +/- .010 tolerance. I sheared the part using a tape measure to size it, punched the holes on a manual one station punch and then proceeded to form the part on a hand brake. I worked and worked on this part trying to get it within the goal tolerance. An hour or two passed and even though I had a nice looking part it was still not within tolerance. I was starting on my second attempt when the foreman came over and asked me what the h**l I was doing. When I explained that I was having a hard time holding the part to +/- .010 he laughed and said that the part was not critical and as long as it was within an 1/8” of an inch it was good enough! If there is a lesson in that story it is this; know what the tolerance is before you waste a lot of time.

The factors that come into play in sheet metal are numerous but let’s just look at one now.
Material thickness: Take a look at the mill tolerances of sheet stock and you will see that the range of thickness for a given gauges bottom and top range actually overlap the gauges on either side. In other words a thin 11 gauge could be sold as a thick 12 gauge while a thick 11 gauge could be a thin 10 gauge. Engineers should allow for 5% thickness variation on thickness which would equate to .006 on 11 gauge. And consider that this amount doubles for each bend in the part as the difference will be seen on each side of the bend. Can tighter tolerances be held? Yes but a premium must be realized in order to achieve them. Hole location from the edge of a part can be held to a tighter tolerance but from a bend to a hole is again affected by the material thickness. Today’s modern numeric control punches and lasers have a positional tolerance of .003 to .005 inches so this must be figured in along with the sheet thickness variation. The only way around this would be to place the hole after the forming operation which is costly. So the in effect the tolerance for a hole from a bend is 10% (2 x 5%) or .012 + .005 or .017 inches for 11 gauge material. Some sheet metal shops will also want additional tolerance allowed for material elasticity variations that affect the form dimensions. At Byers we feel that we overcome these variations to some extent by use of custom K-Factors for the different materials. We also try to overcome these variations at the forming operation by varying the bend radius of the part to get the desired result. Engineers, check a sheet metal gauge chart before designing a part. You might be surprised how many times we get designs calling for 11ga but the part is actually designed with a .125 thickness. 11ga is never .125 thick, it is more commonly .120. That’s .005 difference before we even start modeling the part. This difference shows up most when the engineer has some dimensions on the inside of the material and others on the outside of the material. Be consistent, dimension to the inside or the outside but not both.
Since I’m discussing sheet metal gauges I must comment on gauge callouts for non-ferrous materials. Don’t call out for 11ga Aluminum. This is an obsolete and leads to confusion. Don’t be surprised if you get a call about this. Most designers are not even aware that gauges differ between ferrous and non-ferrous material which is why I will always call you and ask you what thickness in inches you actually want. A much better way to spec non-ferrous thickness is to give the decimal equivalent such as .090 or .060. Look at this chart to see the difference between ferrous and non-ferrous gauges

For more information on reasonable sheet metal tolerances see this page:

Everything I’ve said in this posting should be taken with a grain of salt. If you can design you part within these boundaries then you will get a better price on the production. But if tighter tolerances are a must then they can be done but you need to expect to pay a premium for them.