SHEETMETAL DESIGN

Sheetmetal design introduction:

Sheet metal is simply metal formed into thin and flat pieces. It is one of the fundamental forms used in metalworking, and can be cut and bent into a variety of different shapes. Countless everyday objects are constructed of the material. Plate, sheet and foils are words used to describe the classification of metal depending upon its thickness. Thicknesses can vary significantly; although extremely thin thicknesses are considered foil or leaf, and pieces thicker than 6 mm (0.25 in) are considered plate. Metal is passed between rolls under extreme pressure to make it thinner and longer in the direction in which it is moving. The amount of pressure that is applied decides which of the three categories the resulting aluminum product will belong.  

Followings are the few characteristic of sheetmetal over machining:

1)      Function:  Most low stress (and many high stress) components requiring moderate stiffness can be created from sheetmetal. Sheetmetal is particularly effective for parts that function as containers, chutes and gates, but can effectively be used for mounting brackets as well.

2)        Attachment method:  Sheetmetal parts are typically welded (permanent), riveted (semipermanent), or connected via fasteners (removable) to other parts. Since sheetmetal parts are typically too thin to be threaded (i.e. too thin to achieve the required 5 threads of engagement), attachment holes should be designed as thru holes.

3)       Mechanical properties: Sheetmetal parts are typically lighter than their billet machined counterparts. In general, simple sheetmetal parts require looser tolerances and are less stiff. Sheetmetal parts requiring welding should be created from steel, because thin aluminum is much more difficult to weld (because of its higher thermal conductivity).

4)       Manufacturing properties:  Sheetmetal parts are typically cheaper and faster to produce than their billet machined counterparts.

More things to be known about sheetmetal design:

·         The raw material for sheet metal manufacturing processes is the output of the rolling process. Typically, sheets of metal are sold as flat, rectangular sheets of standard size. If the sheets are thin and very long, they may be in the form of rolls. Therefore the first step in any sheet metal process is to cut the correct shape and sized ‘blank’ from larger sheet.

·          Design of sheet metal components should be such that it would minimize scrap loss and die cost, and improve efficiency

·         The cost in sheet metal forming operation can be reduced by using thinner sheets if the strength and rigidity are increased by bending and forming into ribs configuration

·         Major considerations for the metal selection are the types of metal and their thickness. Protocase Inc. offers carbon steel and stainless steel as standard offerings

Thumb Rules:

      Design for manufacturability is a very useful concept in today’s sheet metal design industry. A sheet metal design should ideally take care about all the aspects of sheet metal manufacturability. Followings are the important thumb rule in sheet metal design.

      Bend Relief:Bend relief is the notch that needs to be created for sheet metal bending. The flange which does not have relief will result in a greater amount of distortion or tearing of the adjacent material. To prevent tearing relief should provide at bend. As per sheet metal design thumb rules, the length of bend relief should be greater than or equal to the inside bend radius of the bend and the width of the bend relief should be greater than or equal to the sheet metal thickness.

  

     Minimum Hole Size for Sheet Metal: While placing the holes in your drawing please keep in mind that, you should not make holes small enough to break the tool. As you reduce the size of the sheet metal hole, smaller size punches will be required. If the size of the punch becomes too small it may break during operation.The diameter of the hole should be equal or more than the thickness of the sheet metal.

Minimum Clearance Between a Hole and Bend: It is very important to maintain enough clearance between a hole and bend for sheet metal design, or else the hole will get deformed.The distance between the sheet metal bend line and edge of the hole should be equal or  greater than four time thickness of the sheet metal

     Minimum Sheet Metal Bending Radius: Minimum sheet metal bend radius depends on the selection of tool and the process. The more ductile the sheet metal, the smaller the inner bend radius is possible.The minimum bend radius for mild steel sheetmetal should be equal to the thickness of Sheetmetal. But for harder material it’s difficult to achieve result in rupture takes place at outer setback. 

 Minimum Flange Width: Minimum flange width should be equal or more than four times sheetmetal thickness. Otherwise, the tool will create marks on the sheet metal surface while manufacturing. 

   

     Bend should be perpendicular to the sheetmetal grains, parallel to grain results in tendency to crack. If bend perpendicular to grain not possible, prefer for 45° to the grain direction.

Bends:

• The minimum flange length is based on the die used to bend.  

• The minimum height of a bent flange is directly related to the material thickness, bend radius, and length of bend.

• Two Bend with same direction results in good accuracy and reduces setup timing. Bends should be tolerance  +/-1.5° at a location adjacent to the bends

• Avoid large parts with small or detailed flanges, which reducing part accuracy.

• Always consult a tooling profile chart when developing your part.  Know the tools available in your shop or the standards if you are outsourcing production.  Specialized tooling can be very expensive.

Counterbores & Countersinks:

While thinner gauge sheets won’t often be countersunk there are a few guidelines to try and follow on thicker sheets to preserve the strength of the sheet and prevent deformation of the features during forming.

• The distance between two countersinks should be kept to at least 8 times the material thickness.

• To ensure strength the distance between a countersink’s edge and the edge of the material should be 4 times the material thickness.

• There should be at least 50% contact between the fastener and the surface of the countersink.

• To prevent any deformation of the hole the edge of the countersink should be at least 4 times the material thickness from the tangent point of the bend.

• The maximum depth is 3 times the material thickness at an angle of the hardware.

Curls:

• The outside radius of a curl can be no smaller than 2 times the material thickness.  

• A hole should be at least the radius of the curl plus material thickness from the curl feature.

Dimples:

• The diameter of a dimple should be no more than 6 times the material thickness.

• The minimum distance between Dimple edge and Hole edge should kept 3 times the material thickness 

• From the part’s edge, dimples edge should be at least 4 times material thickness

• From a bend edge, dimples edge should be at least 3 times material thickness.

• Distance between two dimples should be 4 times material thickness plus the inside radius of each dimple.

• The maximum diameter should be six times the material thickness, and a maximum depth of one-half the inside diameter.

• The minimum distance that a dimple should be from a hole is three times the material thickness plus the radius of the dimple.

• The minimum distance that a dimple should be from the edge is four times the material thickness plus the inside radius of the dimple.

• The minimum distance that a dimple should be from a bend is two times the material thickness plus the inside radius of the dimple plus the radius of the bend.

Gussets

Gussets are used to strengthen a flange; following are the guide lines for gussets.

• 45° gussets shouldn’t be designed to be more than 4 times material thickness on their flat edge

• For holes, the distance between the gusset and the hole’s edge should be at least 8 times material thickness.

• The width and depth, recommended at an angle of 45 degrees, is directly proportional to the radius and material thickness

Hems:

Hems are used to create folds in sheet metal in order to stiffen edges and create an edge safe to touch.

• For tear drop hems, the inside diameter should be equal to the material thickness.

• For open hems, the bend will lose its roundness when the inside diameter is greater than the material thickness.

• For holes, the minimum distance between the hole’s edge and Hem is 3 times the material thickness plus the hem’s radius.

• For bends, the minimum distance between the inside edge of the bend and the outside of the hem should be 5 times material thickness plus bend radius plus hem radius.

Lances & Louvers

Formed lances and louvers will almost always require specialized tooling so be sure to understand what is available to you before designing the feature.

• The minimum depth of a lance should be twice the material thickness and at least .125”

• From a bend, lances edge should be at least 3 times material thickness plus bend radius, however the actual minimum is often much greater than this and driven by the tooling profile.

• From a hole, lances edge should be at least 3 time material thickness from the edge of the hole.

• The minimum width of an open lance is two times the material thickness or 3.00 mm (0.125 inch), 

• The minimum width of a closed lance is two times the material thickness or 1.60 mm (0.06 inch),.

Notches & Reliefs:

• The minimum width of a notch is equal to the material thickness and at least .04”. .

• When determining the length of a notch it is very important to understand the tooling used to cut the notch.  When possible the notch should be equal to a multiple of the punch’s length in order to prevent nibbling from occurring.

• When fabricating with a Punch Press the minimum space between two notches should be at least 2 time material thickness and at least .125”

• The maximum length for a straight/radius end notch is equal to five times the width.

• The maximum length for a V notch is equal to two times the width.

• The minimum distance from a notch to a bend in a parallel plane is eight times the material thickness plus the radius of the bend.

• The minimum distance from a notch to a bend in a perpendicular plane is three times the material thickness plus the radius of the bend.

• The minimum distance between two notches is two times the material thickness or  3.200 mm (0.125 inch)

Equations In Sheetmetal Design:

K-Factor – The ratio of the position of the Neutral Axis to the Material Thickness

Bend Allowance (BA) – It is used to calculate the total length of flat pattern. In other word, Bending allowance is an additional sheet length which given at bend portion. We can get equation of BA by following assumptions,,

BA=arc length, 

Arc length of any bend= (angle in rad) X (radius of neutral axis)

Bend Deduction (BD) – The amount removed from the sum of the two flange lengths to obtain a flat pattern.

Outside Setback (OSSB) – Distance between the outside tangent points and the apex of the outside mold lines.

Inside Setback (ISSB) – Distance between the inside tangent points and the apex of the inside mold lines.

Sheet Metal Forming Processes And Process Terminology: 

(Good Designer Should Know About the Manufacturing Process before Start the Actual Design of Product)

      Sheet metals are widely used for industrial and consumer parts because of its capacity for being bent and formed into intricate shapes. Sheet metal parts comprise a large fraction of automotive, agricultural machinery, and aircraft components as well as consumer appliances. Successful sheet metal forming operation depends on the selection of a material with adequate formability, appropriate tooling and design of part, the surface condition of the sheet material, proper lubricants, and the process conditions such as the speed of the forming operation, forces to be applied, etc. A numbers of sheet metal forming processes such as shearing, bending, stretch forming, deep drawing, stretch drawing, press forming, hydroforming etc. used for specific purpose and the requisite shape of the final product.

Sheet metal operations can be classified as follows.

•Shearing operations- Shearing, Blanking, Piercing, Trimming

•Tension operations- Stretch forming.

•Compression operations- Coining, Sizing, Hobbing

•Tension and compression operations- Drawing, Bending, Forming, Embossing

Shearing:

   Irrespective of the size of the part to be produced, the first step involves cutting the sheet into appropriate shape by the process called shearing. Shearing is a generic term which includes stamping, blanking, punching etc. When a long strip is cut into narrower widths between rotary blades, it is called slitting. Blanking is the process where a contoured part is cut between a punch and die in a press. The same process is also used to remove the unwanted part of a sheet, but then the process is referred to punching. Similarly, nibbling, trimming are a few more examples of cutting process using the same principle of shearing process

Piercing :

     Cutting out holes in a blank strip or a semi-finished component using a press tool is called piercing. The cut out piece is scrap or slug.

Bending:

     Bending is the operation of deforming a flat sheet around a straight axis where the neutral plane lies. In this process Metals take a permanent deformation if they are stressed beyond their elastic limits. It is a very common forming process for changing the sheets and plates into channel, drums, tanks, etc. Spring back is a major problem during bending of sheets that occurs due to elastic recovery by the material causing a decrease in the bend angle once the pressure is removed. The springback can be minimized by introducing excess amount of bending so that the finished bending angle is the same after the elastic recovery. However, a careful estimate of the elastic recovery based on the mechanical behavior of the sheet material is necessary to achieve the same.

Stretch Forming:

     It is a method of producing contours in sheet metal. In a pure stretch forming process, the sheet is completely clamped on its circumference and the shape is developed entirely at the expense of the sheet thickness. The die design for stretch forming is very crucial to avoid defects such as excessive thinning and tearing of the formed part. The stretch forming process is extensively used for producing complex contours in aircraft and automotive parts.

Deep Drawing:

      Deep drawing is a sheet metal forming process in which a sheet metal blank is radially drawn into a forming die by the mechanical action of a punch. It is thus a shape transformation process with material retention. The process is considered "deep" drawing when the depth of the drawn part exceeds its diameter. This can be achieved by redrawing the part through a series of dies. The metal flow during deep drawing is extensive and hence, requires careful administration to avoid tearing or fracture and wrinkle. In deep drawing process type of material and thickness plays major role: Slightly thicker materials can be gripped better during the deep drawing process. Also, thicker sheets have more volume and hence can be stretched to a greater extent. However, the drawing force will increase with the sheet thickness. The percentage elongation property or ductility of the material is an essential quality for materials to be used for deep drawing.

Terminology:

• Air Bending – One of the three types of bending for sheet metal where the outside mold line is not pressed against the die.

• Air Bend Force Chart – A chart used to calculate the tonnage required for a bend based on thickness, tooling and length.

• Annealing – Annealing is a treatment for metals where a material is heated above the recrystallization temperature maintained for a period of time and then cooled.  Annealing is used to soften material, relieve internal stresses and improve its cold working properties.

• Bending – The process of cold working metal to achieve a desired profile.

• Bend Line – The line across the metal where the punch comes in contact with the metal and the bend begins.

• Bump Bending – Also known as Step Bending, the process for forming a large radius with conventional tooling by performing a series bends in close proximity.

• Blanking – The process of cutting flat patterns from stock sheeting, done typically with lasers, water jets, plasmas or punch presses.

• Bottom Bending – One of the bending process in sheet metal where the radius of the punch tip is pushed into the sheet metal.

• Box Bending – The process of bending a 4 sided sheet metal box.

• Coining – One of the bending process in sheet metal where the punch penetrates into the sheet metal under high tonnage forming a consistent bend.

• Cross Break – Light bends added to sheet metal in order to stiffen its surface.

• Crowning – The deflection along a bend due to the tooling or brake not being able to apply equal tonnage along the bend.  Crowning is controlled on modern brakes with internal hydraulic systems which can help equalize pressure.

• Curling – A forming process which leaves a circular, closed loop at the end of the sheet.  This forms a safe edge for handling and stiffens the part’s edge.

• Flange Length – The length of the workpiece when measured from the apex to the edge of the bend.

• Flat Pattern – The general term for the unfolded, flattened, geometry of a part.

• Foil – Very thin sheet metal made from typically malleable metals such as aluminum and gold.

• Gage, Gauge – The thickness of the metal organized by numbers, the larger the number the thinner the metal.

• Galvanneal – Steel which has been galvanized and then subsequently annealed.

• Galvanized – In order to prevent rust steel is dipped into molten zinc which alloys itself with the surface of the steel.

• Gusset – A section of the metal inside a bend which is not bent, but rather

forced into the bend in order to stiffen the piece.

• Hem – A flange that reaches 180° or more.  Hems can be flattened, left open or in a variety of tear drop shapes.

• Jog – Also known as an offset bend, this is when two bends of the same angle, but opposite direction, are used to create a ‘z’ shaped profile.

• Kink – A light bend typically between 5° and 15° which is used to stiffen a flat piece of metal.

• Large Radius Bending – Also known as R Bending, large radius bending is when the inside radius is greater than 8 times the material thickness.

• Leg – Length of the work piece from the edge to the outside tangent point of the bend radius.

• Neutral Axis – An imaginary line within the bend where the material goes through no compression or stretching during the bend process.

• Obtuse Angle – A geometry term for an angle which is greater than 90°.

• R Bending – Bending with an inside radius greater than 8 times the material thickness.

• Reflex Angle – A geometry term for an angle which is greater than 180°

• Sharp Bend – When the radius of the bend is less than %63 of the material thickness, seen commonly with hemming applications.

• Spring Back – The amount to which the workpiece resists bending by returning to its original shape.

• Step Bending – Also known as bump bending, the process for forming a large radius with conventional tooling by performing a series bends in close proximity.

• Straight Angle – A geometry term for an angle which is equal to 180°.

• Tolerances – General dimensioning and tolerances of bends and sheet metal.

• Tooling – General term for the dies, punches and holders found on press brake equipment.