Sheet Metal Design and Stretching Process
1.1 Selection of Sheet Metal Materials
Sheet metal is the most commonly used material in the structural design of communication products. Understanding the comprehensive properties of materials and making the correct selection significantly impact product cost, performance, quality, and manufacturability.
1.1.1 Principles of Material Selection for Sheet Metal
1) Use common metal materials and reduce the variety of material specifications, keeping them within the range of the company's material handbook if possible.
2) Minimize the variety of materials and the specifications of sheet thickness within the same product.
3) Under the premise of ensuring the functionality of the parts, choose the cheapest types of materials possible, reduce material consumption, and lower material costs.
4) For cabinets and some large plug-in boxes, it is necessary to consider reducing the overall weight of the machine.
1.1.2 Introduction to Several Commonly Used Sheet Materials
1.1.2.1 Steel Plate
1) Cold Rolled Steel Sheet
Cold rolled steel sheet, abbreviated as carbon structural steel cold-rolled sheet, is made from hot-rolled steel strip of carbon structural steel, further cold rolled into steel plates with a thickness less than 4mm. As it is rolled at room temperature without iron oxide scale, the cold plate has good surface quality, high dimensional accuracy, and its mechanical and process performance are better than those of hot-rolled steel sheets after annealing treatment.
2) Continuous Electro-Galvanized Cold Rolled Steel Sheet
Continuous electro-galvanized cold rolled steel sheet, also known as "electrolytic plate," refers to the process where zinc is continuously deposited on the prepared steel strip surface under the action of an electric field along the galvanizing line. Due to process limitations, the plating is relatively thin.
3) Continuous Hot-Dip Galvanized Steel Sheet
Commonly known as galvanized sheet or tinplate, this is a continuous hot-dip galvanized thin steel sheet and steel strip with a thickness of 0.25~2.5mm. The steel strip is first passed through a preheating furnace heated by flame to burn off the residual oil on the surface and generate an iron oxide film, then enters a reduction annealing furnace with a mixture of H2 and N2 gases heated to 710~920°C to reduce the iron oxide film to sponge iron.
4) Aluminum-Zinc Coated Sheet
The aluminum-zinc alloy coating of the aluminum-zinc coated sheet is composed of 55% aluminum, 43.4% zinc, and 1.6% silicon, solidified at 600°C, forming a dense quaternary crystal protective layer with excellent corrosion resistance. Its normal service life can reach up to 25 years, which is 3-6 times longer than that of galvanized sheets and comparable to stainless steel. The corrosion resistance of the aluminum-zinc coated sheet comes from the protective function of the aluminum barrier layer and the sacrificial protection of zinc.
The above-mentioned 2), 3), and 4) steel plates are collectively referred to as coated steel plates, which are widely used in domestic communication equipment. After processing, these coated steel plates can be used directly without further electroplating or painting, and the cut edges do not require special treatment. They can also undergo special phosphating treatment to improve the rust resistance of the cut edges.
5) Stainless Steel Sheet
Stainless steel is widely used due to its strong corrosion resistance, good electrical conductivity, and high strength. However, its downsides must also be fully considered: the material is expensive, costing four times that of ordinary galvanized sheets; its high strength causes greater wear on the tools of CNC punch presses, generally unsuitable for processing on CNC punch presses; the press-in nuts for stainless steel sheets must use high-strength special stainless steel materials, which are very expensive.
1.1.2.2 Aluminum and Aluminum Alloy Sheets
The commonly used aluminum and aluminum alloy sheets mainly include the following three materials: rust-proof aluminum 3A21, rust-proof aluminum 5A02, and hard aluminum 2A06.
Rust-proof aluminum 3A21, formerly known as LF21, is an AL-Mn alloy and is the most widely used type of rust-proof aluminum. The strength of this alloy is not high (only higher than industrial pure aluminum), and it cannot be strengthened by heat treatment.
Rust-proof aluminum 5A02, formerly known as LF2, is an AL-Mg rust-proof aluminum. Compared with 3A21, 5A02 has higher strength, especially high fatigue strength, plasticity, and corrosion resistance. It cannot be strengthened by heat treatment, has good weldability with contact welding and hydrogen atom welding, but tends to form crystalline cracks during argon arc welding, and the alloy tends to form crystalline cracks during cold work hardening.
Hard aluminum 2A06, formerly known as LY6, is a commonly used hard aluminum grade. Hard aluminum and super-hard aluminum have higher strength and hardness than general aluminum alloys and can be used as materials for some panels. However, their plasticity is poor, and they cannot be bent, as bending can cause cracks or fractures at the outer rounded corners.
Copper and Copper Alloy Sheets
The commonly used copper and copper alloy sheets mainly include two types, red copper T2 and brass H62.
Red copper T2 is the most commonly used pure copper, which has a purplish appearance, also known as red copper. It has high electrical conductivity, thermal conductivity, good corrosion resistance, and formability, but its strength and hardness are much lower than brass, and the price is very expensive. It is mainly used for conductive, thermal, and durable consumer product corrosion components, generally used in parts on the power supply that need to carry large currents.
Brass H62, a high-zinc brass, has higher strength and excellent cold and hot workability, and is easy to carry out various forms of pressure processing and cutting. It is mainly used for various deep drawing and bending stress parts. Its conductivity is not as good as red copper, but it has better strength and hardness, and the price is relatively moderate. When the conductivity requirements are met, brass H62 is used as much as possible instead of red copper.
The Influence of Materials on Sheet Metal Processing Technology
Sheet metal processing mainly includes three types: punching, bending, and stretching. Different processing technologies have different requirements for sheet materials, and the selection of sheet materials for sheet metal should also consider the approximate shape of the product and the processing technology.
1.1.3.1 The Influence of Materials on Punching Processing
Punching requires the sheet material to have sufficient plasticity to ensure that the sheet does not crack during punching. Soft materials (such as pure aluminum, rust-proof aluminum, brass, red copper, low carbon steel, etc.) have good punching performance, and the punched parts can obtain smooth cross-sections and very small bevels; hard materials (such as high carbon steel, stainless steel, hard aluminum, super hard aluminum, etc.) have poor quality after punching, with large unevenness of the cross-section, especially for thick plates.
1.1.3.2 The Influence of Materials on Bending Processing
Sheet materials that need to be bent should have sufficient plasticity and a lower yield limit. Materials with high plasticity are not easy to crack during bending, and materials with a lower yield limit and lower modulus of elasticity have small rebound deformation after bending, making it easy to obtain dimensionally accurate bent shapes. Materials with good plasticity such as low carbon steel with carbon content <0.2%, brass, and aluminum are easy to bend; brittle materials, such as phosphor bronze (QSn6.5-2.5), spring steel (65Mn), hard aluminum, super hard aluminum, etc., must have a large relative bending radius (r/t) when bending, otherwise, they are prone to cracking during the bending process.
1.1.3.3 The Influence of Materials on Stretching Processing
Stretching of sheet material, especially deep drawing, is one of the more difficult types of sheet metal processing technology. It not only requires the depth of stretching to be as small as possible, the shape to be as simple and smooth as possible, but also requires the material to have good plasticity; otherwise, it is very easy to cause overall distortion, local wrinkling, or even tearing at the stretched parts. The lower the yield strength and the greater the thickness directionality coefficient, the smaller the ratio of yield strength to tensile strength (σs/σb), the better the stamping performance, and the greater the limit of one-time deformation. When the thickness directionality coefficient is >1, the deformation in the width direction is easier than in the thickness direction. The larger the stretching corner radius R value, the less likely it is to produce thinning and breakage during the stretching process, and the better the stretching performance.
1.1.3.4 The Influence of Materials on Stiffness
In the design of sheet metal structures, it is often encountered that the stiffness of the sheet metal components cannot meet the requirements. Designers often use high carbon steel or stainless steel instead of low carbon steel, or hard aluminum alloys with higher strength and hardness instead of ordinary aluminum alloys, hoping to improve the stiffness of the parts, but in fact, there is no obvious effect. For the same base material, the strength and hardness can be greatly improved through heat treatment and alloying, but the change in stiffness is very small. To improve the stiffness of the parts, it is necessary to change the material or the shape of the parts.
1.1.3.5 Performance Comparison of Common Sheet Materials
Table 1-3 Performance comparison of several common sheet materials
Punching and Blanking:
1.2.1 Common Methods of Punching and Blanking
1.2.1.1 CNC Punching and Blanking:
CNC punching and blanking involve using a microcomputer on a CNC punch press to pre-input the processing program for sheet metal parts (dimensions, processing paths, processing tools, etc.), allowing the CNC punch press to use various tools to achieve various forms of processing such as punching, edge cutting, and forming through rich NC instructions. CNC punching generally cannot achieve punching and blanking of shapes that are too complicated. Features: fast speed, saves on molds. Processing is flexible and convenient. It can basically meet the needs of sample production. Issues and requirements to note: Thin materials (t<0.6) are difficult to process, and the material is prone to deformation; the processing range is limited by tools, clamps, etc.; moderate hardness and toughness have better punching performance; too high hardness increases the punching force, which has a negative impact on the punch and precision; too low hardness causes serious deformation during punching, greatly limiting precision; high plasticity is advantageous for forming processing but is not suitable for nibbling, continuous punching, and also not quite appropriate for punching and edge cutting.
CNC punching is generally suitable for punching low carbon steel, electrolytic plates, aluminum-zinc plated sheets, aluminum sheets, copper sheets with T=3.5～4mm or less, and stainless steel sheets with T=3mm or less. The recommended thickness of sheet material for CNC punching is: 0.8～4.0 for aluminum alloy and copper sheets, 0.8～3.5mm for low carbon steel sheets, and 0.8～2.5mm for stainless steel sheets.
The diameter and width of the tool used in stamping must be greater than the thickness of the material, for example, a Φ1.5 tool cannot punch material that is 1.6mm thick. Materials below 0.6mm are generally not processed with NCT.
Stainless steel materials are generally not processed with NCT. (Of course, materials between 0.6~1.5mm can be processed with NCT, but it causes significant tool wear, and the rate of defective products during on-site processing is much higher than for other materials like GI.)
Other shapes of punching and blanking should be as simple and uniform as possible.
Cold Stamping for Punching and Blanking:
For parts with large production volumes and not too large dimensions, punching and blanking are carried out using specially designed sheet metal stamping dies to improve production efficiency. These are generally composed of male and female dies. The female die types include: inlay type and splicing type, etc. Male die types include: round, replaceable; combination type; quick-change type, etc. The most common types of dies are: blanking die (mainly include: open blanking die, closed blanking die, punch-blanking compound die, open punch-blanking progressive die, closed punch-blanking progressive die), bending die, drawing die.
Features: Because cold stamping dies can complete punching and blanking in one stamping operation, they are efficient, consistent, and low-cost. Therefore, for parts with an annual processing volume of over 5,000 pieces and not too large in size, manufacturers generally use cold stamping dies for processing, and the structural design should consider the process characteristics of cold stamping die processing.
Dense Hole Punching:
Dense hole punching can be seen as a type of CNC punching. For parts with a large number of dense holes, to improve punching efficiency and accuracy, a punching die that can punch a large number of dense holes at once is specially developed for processing the workpiece.
Considerations and requirements for dense hole design:
The design of dense holes on the product should consider the processing characteristics of the dense hole punching die, which is to repeat punching multiple times. Therefore, when designing the arrangement of dense holes, the following principles should be adopted:
1) When designing the arrangement of dense holes, first consider using the dense hole dies planned in the "Sheet Metal Die Handbook" to reduce die costs;
2) The arrangement of the same type of dense holes should be uniform, with a fixed value for the row spacing and a fixed value for the column spacing, so that the same type of dense hole dies can be used universally, reducing the number of dies required and lowering the cost of the dies;
3) The size of the same type of holes should be consistent, such as hexagonal holes unified to an inscribed circle Φ5 hexagonal hole, which is the common size for the company's hexagonal holes, accounting for more than 90% of the hexagonal dense holes.
4) When using a staggered arrangement with unequal numbers of holes in two rows, two requirements must be met:
a. The hole spacing must be large, with the edge distance between two holes greater than 2t (t is the material thickness);
b. The total number of rows should be an even number;
5) If the distance between dense holes is very small and the number of holes per row must be even, when the distance D between two dense holes is less than 2t (t is the material thickness) due to the strength of the die, the dense hole die must be set intermittently. The shaded part in the diagram represents the dense hole die. It can be seen that the number of holes per row must be even. If the distance between the holes in the middle is also very small and the number of holes per row is not equal (7 holes, 8 holes two kinds), then it is not possible to punch out all at once with a dense hole die.
When designing the arrangement of dense holes, try to design according to the above requirements, and make them continuous and regular to facilitate the development of dense hole dies, reduce stamping costs, otherwise, CNC punching or many sets of dies must be used to complete the processing.
Staggered holes, the number of rows is not even; missing holes in the middle; the distance between dense holes is too close, the number of holes per row and column is odd, the distance between dense holes is too close, and the number of holes per row in dense holes is not equal. These cannot be completed in one punch with a dense hole die and must be supplemented with other processing methods to complete.
Laser Cutting:
Laser cutting is a non-contact cutting technology that uses electronic discharge as the energy supply and focuses a laser beam as a heat source using a set of reflectors. This high-density light energy is used to achieve punching and blanking of sheet metal parts.
Features: A variety of cutting shapes, faster than wire cutting, small heat-affected zone, no material deformation, fine cuts, high precision and quality, low noise, no tool wear, no need to consider the hardness of the cutting material, can process large, complex shapes and other parts that are difficult to process by other methods.
Issues and requirements to note: Generally only used for steel plates. Aluminum and copper plates are generally not used because the material conducts heat too quickly, causing melting around the cut and cannot guarantee processing precision and quality.
Wire Cutting:
Wire cutting is a machining method that uses the workpiece and electrode wire (molybdenum wire, copper wire) as poles and maintains a certain distance. When there is a sufficiently high voltage, a spark gap is formed to erode the workpiece, and the removed material is carried away by the working fluid.
Features: High machining precision, but slower processing speed, higher cost, and it changes the surface properties of the material. Generally used for mold processing, not for producing parts. Some single-board profile panels have square holes without rounded corners, which cannot be milled, and because aluminum alloys cannot be cut with lasers, if there is no space for punching, wire cutting must be used, which is very slow and inefficient.
Comparison of the Characteristics of Three Common Blanking and Punching Methods:
Technological Design of Punching and Blanking:
1.2.2.1 Technological Design of Arrangement
For mass and medium-volume production, the cost of material takes up a significant proportion. The full and effective use of materials is an important economic indicator in sheet metal production. Therefore, without affecting the usage requirements, the structural designers strive to adopt a layout method that has no or minimal waste.
1.2.2.2 Technological Nature of Blanking Parts
For CNC punching machines processing external fillets, specialized external round tools are required. To reduce the number of external round tools, as shown in Figure 1-9, this manual standardizes external fillet radii as:
1) 90-degree right-angle external fillets with radii of r2.0, r3.0, r5.0, r10.
2) 135-degree oblique angle external fillets uniformly at R5.0.
Priority is given to using round holes for punching, and round holes should be selected according to the series specified in the "Sheet Metal Die Handbook." This can reduce the number of round hole tools and the time it takes for CNC punching machines to change tools.
Due to the strength limitations of the punching convex die, the hole diameter cannot be too small, and the minimum hole diameter is related to the material thickness. When designing, the minimum diameter of the hole should not be less than the values shown in Table 1-5 below.
Considering that in the die stamping process, the precision between holes and the outer shape, and between holes processed with a compound die, is easier to ensure, and the processing efficiency is higher, and considering the maintenance cost and convenience of the die, the distance between holes, and between holes and the outer shape, if it can meet the minimum wall thickness requirements of the compound die, the processability is better.
When punching holes on deep-drawn parts, as shown in Figure 1-13, to ensure the shape and positional accuracy of the holes and the strength of the die, a certain distance should be maintained between the hole wall and the straight wall of the part, i.e., the distances a1 and a2 should meet the following requirements: a1 ≥ R1 + 0.5t, a2 ≥ R2 + 0.5t, where R1, R2 are the fillet radii.
1.2.2.3 Processing Precision of Blanking Parts
Principles for selecting the design dimension datum for stamping parts:
1) The design dimension datum for stamping parts should coincide as much as possible with the manufacturing positioning datum to avoid manufacturing errors in dimensions.
2) The hole position dimension datum for stamping parts should be chosen as much as possible on surfaces or lines that do not undergo deformation from beginning to end in the punching process and should not be connected with parts that undergo deformation.
3) For parts that are punched in multiple steps on different dies, it is best to use the same positioning datum.
1.2.2.4 Secondary Cutting
Secondary cutting, also called secondary blanking or trimming (very poor processability, should be avoided in design), refers to the process where stretched features deform the material by extrusion, or when bending deformation is significant, increasing the blanking size, first forming, then trimming holes or the outer contour to remove reserved material and obtain the correct complete structural dimensions.
Application: Trimming is necessary when features such as stretched bosses are close to the edge. Taking countersinking as an example to illustrate,
1.3 Bending of Sheet Metal Parts
Bending of sheet metal refers to the process of changing the angle of a sheet or part, such as bending a sheet into a V-shape or U-shape. Generally, there are two methods of sheet metal bending: one method is die bending, used for sheet metal structures that are relatively complex, small in size, and mass-produced; the other is bending machine bending, used for processing sheet metal structures that are larger in size or not produced in large quantities.
These two bending methods have their principles, characteristics, and applicability.
1.3.1 Die Bending:
For structural parts with an annual processing volume of over 5,000 pieces and not too large in size (generally 300x300), manufacturers usually consider using stamping dies for processing.
1.3.1.1 Common Bending Dies
To extend the life of bending dies, parts should be designed with rounded corners whenever possible.
With too small a flange height, even using bending dies is not conducive to forming; generally, the flange height L should be at least 3t (including wall thickness).
1.3.1.2 Processing Methods for Steps
For bending low-height Z-shaped steps in sheet metal, manufacturers often use simple dies on punch presses or hydraulic presses. For small batches, it can also be processed on a bending machine with a stepped die, as shown in Figure 1-18. However, the height H should not be too high, generally within (0–1.0)t. If the height is (1.0–4.0)t, the use of a die with a loading and unloading structure should be considered based on the actual situation. The height of the step in such a die can be adjusted by adding shims, so the height H is adjustable. However, there is a drawback: the length L is not easy to ensure, and the perpendicularity of the vertical side is not easy to guarantee.
1.3.2 Bending Machine Bending
Bending machines are divided into ordinary bending machines and CNC bending machines. Due to the high precision requirements and irregular bending shapes, the sheet metal bending for communication equipment is generally done using CNC bending machines. The basic principle is to use the bending tools (upper die) and V-shaped grooves (lower die) of the bending machine to bend and form the sheet metal.
1) Bending Tools (Upper Die)
The tools are mainly selected based on the shape of the workpiece during processing. Generally, manufacturers have a variety of shapes for bending tools, especially those with a high degree of specialization, who custom-make many shapes and specifications of bending tools for processing various complex bends.
2) The lower die generally uses a V=6t (t is the material thickness) die.
There are many factors that affect bending processing, mainly including the upper die radius, material, material thickness, lower die strength, and the size of the die opening. To meet product needs and ensure the safe use of bending machines, manufacturers have standardized the bending die series. During the structural design process, we need to have a general understanding of the existing bending dies.
Basic principles for the sequence of bending processing:
1) Bend from inside to outside;
2) Bend from small to large;
3) First bend special shapes, then bend general shapes;
4) Ensure that the previous operations do not affect or interfere with subsequent ones.
1.3.2.2 Bending Radius
When bending sheet metal, a bending radius is required at the bend. The bending radius should not be too large or too small and should be appropriately selected. A too small bending radius can easily cause cracking at the bend, while a too large bending radius can make the bend prone to springback. The preferred bending radius (inner radius of the bend) for different materials and thicknesses:
The data in the above table are preferred values and are for reference only. In reality, the radius of the bending tools used by manufacturers is usually 0.3, with a few bending tools having a radius of 0.5, so the inner fillet radius of our sheet metal bends is basically 0.2. For ordinary low-carbon steel plates, rust-proof aluminum plates, brass plates, copper plates, etc., an inner fillet radius of 0.2 is not a problem. However, for some high-carbon steels, hard aluminum, or super hard aluminum, such bending radii can lead to bending fractures or cracking at the external fillet.
1.3.2.3 Bending Springback
3) Factors affecting springback and measures to reduce it.
1. The magnitude of the springback angle is directly proportional to the material's yield point and inversely proportional to the elastic modulus E.
For sheet metal parts with high precision requirements, to reduce springback, materials should be chosen as low carbon steel whenever possible, instead of high carbon steel or stainless steel.
2. The larger the relative bending radius r/t, the less the deformation, and the larger the springback angle Δα. This is an important concept; the corner radius in sheet metal bending should be as small as possible within the limits of material properties to improve accuracy. Particularly, designing large arcs should be avoided as much as possible, as such large arcs pose significant challenges to production and quality control:
1.3.2.4 Calculation of the Minimum Bending Edge for Single Bending
An important parameter here is the width B of the lower die opening. Considering the bending effect and die strength, there exists a minimum required width of the die opening for materials of different thicknesses. Below this value, problems may arise such as incomplete bending or damage to the die.
Note: 1. The minimum bending height includes one material thickness.
2. When V-bending is to form a sharp angle, the shortest bending edge needs to be increased by 0.5.
3. When the part material is aluminum or stainless steel plate, the minimum bending height will change slightly, decreasing for aluminum and increasing for stainless steel, as referenced in the above table.
1.3.2.5 Minimum Bending Height for Z-shaped Bends
The process for Z-shaped bends is very similar to that for L-shaped bends, also presenting issues with the minimum bending edge. Due to the structure limitation of the lower die, the shortest side for Z-shaped bends is greater than for L-shaped bends. The formula for calculating the minimum side of Z-shaped bends is:
1.3.2.6 Interference During Bending
For secondary or more complex bends, interference often occurs between the workpiece and the tool, as shown in Figure 1-27, where the black part indicates interference. This makes bending impossible, or the interference may cause deformation during bending.
The interference issue in sheet metal bending is not too technical; it simply requires an understanding of the shape and size of the bending die. The common shapes of bending tool cross-sections are introduced in the newly revised "Sheet Metal Die Handbook," and corresponding tool entities are available in the intralink library. If unsure during design, one can follow the principle shown in the diagram and use the tool for assembly interference checks directly.
For tapping after forming a hole, as shown in Figure 1-29, the D value cannot be designed too small. The minimum D value can be calculated or determined by drawing, based on material thickness, forming hole outer diameter, forming hole height, and chosen bending tool parameters.
1.3.2.7 Minimum Distance from Holes, Long Slots to Bending Edge
Holes or slots too close to the bending line can't lift the material during bending, causing deformation of the hole shape; therefore, the distance from the hole edge to the bending line should be greater than the minimum edge distance X≥t+R.
For long slots too close to the bending line, the same problem occurs. Therefore, the distance from the slot edge to the bending line should be greater than the minimum edge distance according to Table 1-14, with bending radii referred from Table 1-9.
1.3.2.8 Special Processing Treatment When Holes Are Close to the Bend
When holes near the bend line are closer than the minimum distance mentioned above, deformation will occur after bending. Depending on different product requirements, the following treatments as shown in Table 1-15 can be applied. However, these methods are less desirable from a processing perspective, and structural design should avoid these situations whenever possible.
1.3.2.9 Process Holes, Slots, and Notches for Bent Parts
In the design of bent parts, if it is necessary to bend the flange into the blank's inner edge, process holes, slots, or notches should generally be punched after blanking.
d - Diameter of the process hole, d≥t; K - Width of the process notch, K≥t.
Crack stop slots or notches: Generally, for bending only part of an edge, to avoid tearing and distortion, crack stop slots or notches should be made. This is especially necessary for bends with internal angles less than 60 degrees. The width of the notch should generally be greater than the material thickness t, and the depth should generally be greater than 1.5t.
Process slots and holes must be properly handled. Panels and externally visible parts may avoid adding process holes for bending (for example, panels may not have process notches to maintain a uniform style), but other parts should include process holes for bending corners.
1.3.2.10 Clearance for 90-Degree Directional Bends:
During drawing design, clearances for 90-degree directional bends should not be marked unless specifically required, as some unreasonable clearances can affect the processing design of manufacturers. Manufacturers usually design the process with a clearance of 0.2 to 0.3.
1.3.2.11 Bending at Transition Points
The bending area of bent parts should avoid the locations of abrupt changes in the part. The distance L from the bend line to the deformation zone should be greater than the bending radius r.
1.3.2.12 Single Hit Dead Edge
The method for a single hit dead edge: First, bend the sheet to 30 degrees with a 30-degree bending tool, then flatten the bent edge.
The minimum bending edge size L should be calculated as the minimum bending edge size for a single bend described in 1.3.2.2 plus 0.5t (t for material thickness). Dead edging is generally suitable for sheet materials such as stainless steel, galvanized sheet, and aluminum-zinc plated sheet. It is not suitable for plated parts because there can be acid entrapment at the dead edge.
1.3.2.13 180-Degree Bending:
The method for 180-degree bending: First, bend the sheet to 30 degrees with a 30-degree bending tool, then flatten the bend and remove the shim after flattening.
1.3.2.14 Triple Folding Dead Edge:
First form the shape, then fold the dead edge. During design, pay attention to the dimensions of each part to ensure that all processing steps meet the minimum bending dimensions to avoid unnecessary post-processing.
1.4 Nut and Screw Structures on Sheet Metal Parts
1.4.1 Riveted Nuts
Common forms of riveted nuts include press-riveted nut studs, press-riveted nuts, expand-riveted nuts, pull-riveted nuts, and floating press-riveted nuts.
1.4.1.1 Press-Riveted Nut Studs
Press-riveting refers to the process where, under external pressure, the riveting part causes plastic deformation of the base material and is squeezed into a specially designed pre-made groove in the screw/nut structure, thereby achieving reliable connection of two parts. There are two types of non-standard nuts for press-riveting: press-riveted nut studs and press-riveted nuts. This type of riveting usually requires the hardness of the riveting parts to be greater than that of the base material. Common low-carbon steel, aluminum alloy, and copper sheets are suitable for press-riveted nut studs. For stainless steel and high-carbon steel sheets, because the material is harder, specially made high-strength press-riveted nut studs are required, which are not only expensive but also difficult to press firmly, and may easily fall off after pressing. To ensure reliability, manufacturers often need to weld on the side of the nut stud, which is not a good process. Therefore, sheet metal parts with press-riveted nut studs and press-riveted nuts should avoid using stainless steel as much as possible.
1.4.1.3 Expand-Riveted Nuts
Expand-riveting refers to the process where, during riveting, part of the material of the screw or nut deforms plastically under the action of external force and forms a tight fit with the base material, thereby achieving reliable connection of the two parts. Commonly used expand-riveted nuts like ZRS are connected to the base material using this type of riveting.
1.4.1.4 Pull-Riveted Nuts
1) Pull-riveting refers to the process where, during riveting, the riveting part deforms plastically under the action of external pulling force, and the deformation usually occurs at a specially designed location, clamping the base material to achieve a reliable connection. Commonly used pull-riveted nuts are connected to the base material using this type of riveting. Pull-riveting is done with a special rivet gun and is often used where installation space is limited and generic riveting tools cannot be used.
1.4.1.5 Floating Press-Riveted Nuts
Some sheet metal structures require riveted nuts, and due to the complexity of the overall chassis structure and large cumulative structural errors, the relative positional accuracy of these riveted nuts can be significantly off, leading to difficulties in assembling other parts. The use of floating press-riveted nuts at the corresponding press-riveted nut positions has greatly improved this situation.
1.4.1.6 Distance from Expand-Riveted or Press-Riveted Nuts to the Edge
Both expand-riveted and press-riveted nuts are joined to the sheet metal by squeezing the material, if the distance to the edge is too close, it can easily deform this area. Unless there are special requirements, the minimum distance from the centerline of the riveted fastener to the edge of the plate should be greater than L.
1.4.1.7 Factors Affecting Riveting Quality
There are many factors that affect the quality of riveting. The main ones are summarized as follows: base material properties, pilot hole size, and riveting method.
1) Base material properties. When the hardness of the base material is appropriate, the quality of riveting is good, and the riveted part can withstand forces well.
2) Pilot hole size. The size of the pilot hole directly affects the quality of riveting. If it is too large, there will be a significant gap between the base material and the riveted part. For press-riveting, there won't be enough deformation to fill the grooves on the riveted part, resulting in insufficient shear force and directly affecting the push-out resistance of the press-riveted nut (or stud). For expand-riveting, if the pilot hole is too large, the compressive force generated by plastic deformation during riveting is reduced, directly affecting the push-out and torsion resistance of the expand-riveted nut (or screw). The same applies to pull-riveting; a too-large pilot hole reduces the effective friction force between the two parts after plastic deformation, affecting the quality of riveting.
3) Riveting method. This has already been introduced in the previous section.
Care must be taken when using riveted screws and nuts, as different applications and force requirements will necessitate different types of fasteners. If an inappropriate type is used, it can reduce the range of forces that the riveted screw or nut can withstand, leading to connection failure.
1) Do not install steel or stainless steel riveted fasteners on aluminum plates before anodic oxidation or surface treatment.
2) Press-riveting too many fasteners in a straight line can cause a buildup of material with nowhere to flow, creating significant stress and causing the workpiece to bend into an arc.
3) Ensure that riveted fasteners are installed after any surface plating treatment on the plate.
4) Nuts sized M5, M6, M8, M10 generally require spot welding, as larger nuts often require greater strength and may use arc welding. For M4 (including M4) and smaller, expand-riveted nuts are preferred; if the part is plated, un-plated expand-riveted nuts may be used.
5) When press-riveting nuts on a bent edge, to ensure the quality of riveting, it is necessary to: 1) ensure that the distance from the rivet hole edge to the bent edge is greater than the deformation zone of the bend, and 2) the distance from the center of the riveted nut to the inside of the bent edge, L, should be greater than the sum of the outer radius of the riveted nut and the inner radius of the bend.
1.4.2 Projection Weld Nuts
Projection weld nuts (spot weld nuts) are very widely used in the design of sheet metal parts and are often used in our company's structural designs. However, in many designs, the size of the pre-hole does not follow standards and cannot be accurately positioned. There are two types of national standard projection weld nuts: one is the welded hex nut GB13680-92, which has relatively coarse positioning and inaccurate dimensions, often requiring re-threading after welding; the other is the welded hex nut GB13681-92, which has a self-positioning structure during welding and is recommended for use. The recommended values for the pre-welding hole diameter D0 and plate thickness H are in accordance with the specifications of Table 1-17.
1.4.3 Tapping after Drilling
List of pre-hole size, outer diameter, height, etc., for tapping after drilling:
1.4.3.1 Common coarse thread tapping sizes
1.4.3.2 Minimum distance from tapping to the bending edge
Table of distances from the center of tapping to the bending edge (H value):
1.4.4 Comparison of swage nuts, press-in nuts, riveting, and tapping after drilling
1.5 Sheet Metal Stretching
1.5.1 Common forms of stretching and design considerations
Considerations for stretching sheet metal parts:
1. The minimum fillet radius between the bottom and the wall of the stretched part should be greater than the thickness of the plate, i.e., \(r1 > t\); to facilitate smoother stretching, it's generally taken as \(r1 = (3 \sim 5)t\), with the maximum fillet radius being less than 8 times the plate thickness, i.e., \(r1 < 8t\).
2. The minimum fillet radius between the flange and the wall of the stretched part should be more than twice the plate thickness, i.e., \(r2 > 2t\); for smoother stretching, it's usually set to \(r2 = 5t\), with the maximum fillet radius being less than 8 times the plate thickness, i.e., \(r1 < 8t\).
3. The inner diameter of circular stretched parts should be \(D \geq d + 12t\) to prevent wrinkling when pressed during stretching.
4. The minimum fillet radius between adjacent walls of rectangular stretched parts should be \(r3 \geq 3t\); to reduce the number of stretches, it is advisable to take \(r3 \geq 1/5H\) for completing the stretch in one go.
5. Due to different stresses in various parts of the stretched piece, the material thickness changes after stretching. Typically, the center of the bottom maintains its original thickness, the material becomes thinner at the bottom fillet, and thicker near the flange at the top; for rectangular stretched pieces, the material becomes thicker around the corners.
6. For the material thickness of stretched parts, it is generally considered that the thickness of the upper and lower walls will not be the same due to the deformation process (i.e., thicker on top, thinner below).
1.5.2 Embossing process dimensions
For embossing shapes and dimensions on sheet metal, several series of dimensions are specified in the "Sheet Metal Mold Handbook." Corresponding Form models are available in the Intralink library. When designing, select the dimensions specified in the handbook and directly use the Form molds from the library.
1.5.2.2 Limit dimensions for embossing spacing and edge distance
1.5.3 Local Indentation and Beading
On sheet metal, a half-shear depression with a depth of 0.3 can be punched for the purpose of adhering labels, which can enhance the reliability of the label attachment. The "Sheet Metal Mold Handbook" specifies a series of dimensions corresponding to the nameplates, and the Intralink library contains the corresponding Form models. When designing, one should select according to the handbook's specified dimensions and directly use the molds from the library. This type of half-shear depression has much less deformation than normal stretching, but for parts such as large-area cover plates and bottom plates without bending or with low bending heights, there is still some deformation. Alternative methods:
a) Punching before bending ensures the precision of the L dimension and is convenient for processing. b) and c) If high precision of dimension L is required, it is necessary to process the hole after bending, which is very troublesome and best avoided.
1.6 Other Processes
1.6.1 Extruded Hole Riveting
Extruded hole riveting is a riveting method between sheet metal parts, mainly used for the connection of coated steel plates or stainless steel plates. It involves punching one part and flanging the punched hole on the other part, riveting them together to form a non-detachable connection. Advantages: The flange and straight hole combination has a self-locating function.
1.6.2 Torx Riveting
In sheet metal riveting methods, another method is Torx riveting. The principle is to stack two plates together and use a mold to punch and stretch them, mainly used for connecting coated steel plates or stainless steel plates. It has the advantages of saving energy, being environmentally friendly, and high efficiency. It was previously more commonly used in the enclosures of the telecommunications industry, but quality control in mass production is challenging, and it is now less used and not recommended.
1.7 Standardization of Countersink Dimensions
1.7.1 Screw Countersink Hole Dimensions
The structural dimensions for screw countersink holes should be selected according to the following table. For the countersink seat of countersunk screws, if the plate is thin and it is difficult to ensure both the through-hole d2 and the countersink D, priority should be given to ensuring the through-hole d2.
