Sheet Metal Processing
Sheet metal processing is a comprehensive cold-working process for metal sheets, typically below 6mm in thickness. It involves various techniques such as shearing, punching, bending, welding, riveting, mold forming, and surface treatment. One significant characteristic of sheet metal processing is the uniform thickness of the same part.
Methods of Sheet Metal Processing:
1. Non-mold Processing: This involves using equipment such as CNC punching machines, laser cutting, shearing machines, bending machines, and riveting machines to process sheet metal. It is generally used for sample production or small-batch production, but it has higher costs. The processing cycle is short, and the response is quick.
2. Mold Processing: This method involves using fixed molds to process sheet metal. It typically includes blanking molds and forming molds and is mainly used for large-scale production, resulting in lower costs. The initial mold costs are high, but the quality of the parts is guaranteed. The initial processing cycle is longer due to the high mold costs.
Sheet Metal Processing Workflow:
1. Blanking: CNC punching, laser cutting, shearing machines.
2. Forming - Bending, stretching, punching: Bending machines, punching presses, etc.
3. Other processes: Riveting, threading, etc.
4. Welding: Connecting sheet metal parts.
5. Surface treatment: Powder coating, electroplating, brushing, silk screening, etc.
Sheet Metal Processing Technique - Blanking:
There are several methods for blanking sheet metal, including CNC punching, laser cutting, shearing machines, and mold blanking. Currently, CNC is the commonly used method, while laser cutting is often used in the prototyping stage (it can also process stainless steel sheet metal parts), but it has higher processing costs. Mold blanking is commonly used for large-scale production.
Let's focus on CNC punching as the main method for blanking sheet metal.
CNC punching, also known as turret punch press, can be used for blanking, punching holes, stretching holes, embossing, and louvering, with a processing accuracy of up to +/- 0.1mm.
The applicable sheet thickness for CNC punching is as follows:
- Cold-rolled plate, hot-rolled plate ≤ 4.0mm
- Aluminum plate ≤ 5.0mm
- Stainless steel plate ≤ 2.0mm
Considerations for CNC Punching:
1. Minimum size requirements for punching. The minimum size of a punched hole depends on the shape of the hole, material mechanical properties, and material thickness.
2. Hole spacing and edge distance in CNC punching. The minimum distance between the punched edge of the part and the outer contour should be no less than the material thickness (t) when the edge is not parallel to the part's outer contour. When the edge is parallel, it should be no less than 1.5t.
3. For stretched holes, the minimum distance between the edge of the hole and the edge of the sheet metal is 3T. The minimum distance between two stretched holes is 6T. The minimum safe distance between a stretched hole and a bending edge (inner) is 3T + R (T is the sheet metal thickness, and R is the bending radius).
4. When punching stretched bends and deep-drawn parts, there should be a certain distance between the hole wall and the straight wall.
Sheet Metal Processing Technique - Forming
Forming of sheet metal mainly involves bending and stretching.
1. Sheet Metal Bending
1.1 Bending of sheet metal is primarily done using a bending machine.
Processing accuracy of the bending machine:
Single bend: +/- 0.1mm
Two bends: +/- 0.2mm
More than two bends: +/- 0.3mm
1.2 Basic principles of bending sequence: Bending should be done from the inside to the outside, from small to large, and special shapes should be bent first without affecting or interfering with subsequent processes.
1.3 Common bending tool shapes:
Common V-groove shapes:
1.4 Minimum bending radius for bent parts:
When a material is bent, the outer layer experiences tension, while the inner layer experiences compression. When the material thickness is constant, the smaller the inner radius (r), the more severe the tension and compression of the material. If the tensile stress on the outer layer exceeds the material's ultimate strength, it can lead to cracks and fractures. Therefore, the structural design of bent parts should avoid excessively small bending radii. The minimum bending radii for commonly used materials in the company are shown in the table below.
Table of Minimum Bending Radii for Bent Parts:
The bending radius refers to the inner radius of the bent part, and t is the material thickness.
1.5 Height of straight edges for bent parts:
In general, the minimum height of straight edges should not be too small. The minimum height requirement is h > 2t.
If the height of the straight edge of the bent part needs to be h ≤ 2t, the bending edge height should be increased first, and then machined to the required dimensions after bending. Alternatively, a shallow groove can be machined within the bending deformation zone before bending.
1.6 Minimum height of the straight edge with an inclined angle on the bending edge:
When the bending part has an inclined angle on the side of the bending edge, the minimum height of the side is h = (2 to 4) t > 3mm.
1.7 Edge distance on bent parts:
Edge distance: When punching holes on bent parts before bending, the hole position should be outside the bending deformation zone to avoid deformation of the hole during bending. The distance from the hole wall to the bending edge is shown in the table below.
1.8 Process notches for localized bending:
The bending line of the bent part should avoid locations with sudden dimensional changes. When bending a specific section of the edge, to prevent stress concentration and bending cracks at sharp corners, the bending line can be moved a certain distance away from the dimensional change area, or process grooves or punch process holes. Dimensional requirements: S ≥ R; groove width k ≥ t; groove depth L ≥ t + R + k/2.
1.9 Avoiding the deformation zone for bent edges with beveled sides:
1.10 Design requirements for sheet metal flanges:
The length of the flange is related to the material thickness, and generally, the minimum length of the flange is L ≥ 3.5t + R.
Where t is the material thickness, and R is the minimum inner bending radius before the flange.
1.11 Addition of process positioning holes:
To ensure accurate positioning of the blank in the mold and prevent the blank from shifting during bending, process positioning holes should be added during the design phase. Especially for parts that undergo multiple bending operations, the process holes must serve as the positioning reference to reduce cumulative errors and ensure product quality.
1.12 Consideration of processability when dimensioning bent parts:
a) When punching holes before bending, it is easier to ensure the dimensional accuracy of L, and the processing is convenient.
b) and c) If high dimensional accuracy is required for L, it is necessary to bend first and then process the holes, which is more complicated.
1.13 Influence of springback on bent parts:
Springback in bent parts is influenced by various factors, including material mechanical properties, thickness, bending radius, and positive pressure during bending. The larger the ratio of the inner bending radius to the plate thickness, the greater the springback. Currently, the suppression of springback is mainly achieved through measures taken by manufacturers in mold design. Additionally, improvements in design can reduce springback angles, such as reinforcing ribs in the bending zone, which not only improves the stiffness of the workpiece but also helps suppress springback.
2. Sheet Metal Stretching
Sheet metal stretching is mainly carried out using CNC or general punching methods with various stretching punches or molds.
The shape of the stretching part should be as simple and symmetrical as possible, and it is preferable to complete the forming in one stretch.
For parts that require multiple stretches, surface marks that may occur during the stretching process should be allowed, as long as they meet the assembly requirements.
With the premise of meeting assembly requirements, a certain inclination of the stretching side wall should be allowed.
2.1 Requirements for the radius of curvature between the bottom of the stretching part and the straight wall:
The radius of curvature between the bottom of the stretching part and the straight wall should be greater than the plate thickness, i.e., r1 ≥ t. To facilitate smooth stretching, it is generally taken as r1 = (3 to 5) t. The maximum radius of curvature should be less than or equal to 8 times the plate thickness, i.e., r1 ≤ 8t.
2.2 Radius of curvature between the flange of the stretching part and the wall:
The radius of curvature between the flange of the stretching part and the wall should be greater than twice the plate thickness, i.e., r2 ≥ 2t. To facilitate smooth stretching, it is generally taken as r2 = (5 to 10) t. The maximum radius of the flange should be less than or equal to 8 times the plate thickness, i.e., r2 ≤ 8t.
2.3 Inner cavity diameter of circular stretching parts:
The inner cavity diameter of circular stretching parts should be taken as D ≥ d + 10t to ensure that the pressing plate can be tightly pressed without wrinkling during stretching.
2.4 Radius of curvature between adjacent walls of rectangular stretching parts:
The radius of curvature between adjacent walls of rectangular stretching parts should be taken as r3 ≥ 3t. To reduce the number of stretches, it should be preferably taken as r3 ≥ H/5 to achieve one-time stretching.
2.5 Size relationship between height and diameter of circular non-flanged stretching parts in one forming:
For circular non-flanged stretching parts in one forming, the ratio of height (H) to diameter (d) should be less than or equal to 0.4, i.e., H/d ≤ 0.4.
2.6 Thickness variation of stretching parts:
Due to different stress distribution, the thickness of the material changes after stretching. Generally, the bottom center maintains its original thickness, the material becomes thinner at the bottom corners, and thicker near the top close to the flange. For rectangular stretching parts, the material becomes thicker at the corners.
2.7 Annotation method for dimensions of stretching parts:
When designing stretching products, the dimensions on the product drawing should clearly indicate whether the external dimensions or internal dimensions need to be ensured. It is not appropriate to annotate both internal and external dimensions simultaneously.
2.8 Annotation method for dimensional tolerances of stretching parts:
The dimensional tolerances for the internal radius of concave-convex arcs and the height of cylindrical stretching parts formed in one step are symmetrical deviations on both sides. The deviation value is half of the absolute value of the GB (national standard) 16th-level precision tolerance, with a ± sign.
3. Other Sheet Metal Forming:
Reinforcement ribs - Pressing ribs on sheet metal parts to increase structural rigidity.
Louvers - Louvers are commonly used on various covers or enclosures to provide ventilation and heat dissipation.
Flanged holes (stretched holes) - Used to process threads or improve the rigidity of the hole opening.
3.1 Reinforcement Ribs:
Reinforcement rib structure and size selection:
The maximum dimensions for embossing spacing and embossing edge distance should be selected according to the table.
3.2 Louvers:
The louver forming method involves cutting the material with one edge of the male die, while the rest of the male die simultaneously stretches the material, forming a wavy shape with one side open.
Louver size requirements: a ≥ 4t; b ≥ 6t; h ≤ 5t; L ≥ 24t; r ≥ 0.5t.
3.3 Flanged Holes (Stretched Holes):
There are various forms of flanged holes, and the common one is the flanged hole for internal threading.
Sheet Metal Processing - Other Processes:
- Riveting auxiliary components on sheet metal, such as rivet nuts, rivet studs, and guide pins.
- Tapping threaded holes on sheet metal.
- Welding in sheet metal fabrication. When designing welded sheet metal structures, the principles of "symmetrical arrangement of welds and weld points, avoiding intersections, clusters, and overlaps, interrupting minor welds and weld points, and connecting major welds and weld points" should be followed.
Sheet Metal Welding
Arc Welding
Sufficient welding space should be provided between sheet metal parts, and the maximum welding gap should be between 0.5 to 0.8mm. The weld should be even and smooth.
2. Spot Welding
The welding surface should be flat without wrinkles or springback.
The dimensions for spot welding are as follows:
Spot Weld Spacing
In practical applications, when welding small parts, the data in the table below can be used as a reference.
For welding large-sized parts, the spot spacing can be appropriately increased, generally not less than 40-50mm. In non-stressed areas, the spot spacing can be increased to 70-80mm.
For plate thickness (t), spot diameter (d), minimum spot diameter (dmin), and minimum distance between spots (e), if the plates have different thicknesses, the thinnest plate should be considered.
Number of Layers and Thickness Ratio in Resistance Spot Welding
In resistance spot welding, the number of layers of the plate is generally 2, with a maximum of 3. The thickness ratio between the layers of the weld should be between 1/3 and 3.
If it is necessary to weld 3 layers of plates, the thickness ratio should be checked first. If it is reasonable, the welding can proceed. If it is not reasonable, considerations should be given to creating process holes or gaps. For 2-layer welding, the spot positions should be staggered.
Sheet Metal Processing - Joining Methods
Here, we mainly introduce the joining methods used in sheet metal processing, including riveting, welding (as mentioned above), clinching, and TOX joining.
Riveting:
This type of rivet, commonly known as a pull rivet, is used to join two pieces of sheet metal together. It is called pull riveting.
2. Welding (mentioned above)
3. Clinching:
One component is punched, and the other component has a countersink. They are joined together through clinching to form a non-removable connection.
Advantages: Clinching, combined with its corresponding sink hole, provides positioning functionality. It offers high joint strength and efficient assembly through the use of molds.
4. TOX Joining:
TOX joining involves using a simple punch to press the connecting part into a die. Under further pressure, the material inside the die flows outward. This results in a rounded joint point without sharp edges or burrs, while preserving its corrosion resistance. Even for sheet metal parts with coatings or paint layers, the original rust and corrosion resistance properties are retained because the coatings and paint layers deform and flow along with the material. The material is squeezed to both sides and into the plate adjacent to the die, forming a TOX connection point.
Sheet Metal Processing - Surface Treatment:
Surface treatment of sheet metal serves both protective and decorative purposes. Common surface treatments for sheet metal include powder coating, electroplating (zinc plating), hot-dip galvanizing, surface oxidation, surface brushing, and silk-screen printing.
Before performing surface treatment on sheet metal, the surface should be cleaned to remove oil, rust, welding slag, etc.
Powder Coating:
There are two types of surface coating for sheet metal: liquid paint and powder paint. Powder paint is commonly used. By spraying, electrostatic adsorption, and high-temperature baking, various colors of coatings are applied to the surface of the sheet metal for aesthetic purposes and to enhance corrosion resistance. It is a commonly used surface treatment method.
Note: There may be slight color differences in the coatings applied by different manufacturers. Therefore, for sheet metal of the same color on the same equipment, it is advisable to use coatings from the same manufacturer.
2. Electroplating (Zinc Plating) and Hot-Dip Galvanizing:
Surface zinc plating is a common method for surface corrosion protection of sheet metal and also provides some aesthetic enhancement. Zinc plating can be divided into electroplating and hot-dip galvanizing.
Electroplated zinc has a bright and smooth appearance, with a relatively thin zinc layer, making it commonly used.
Hot-dip galvanizing produces a thicker zinc layer and can form an iron-zinc alloy layer, providing better corrosion resistance than electroplated zinc.
3. Surface Oxidation:
Here, we mainly introduce anodizing of aluminum and aluminum alloys.
Anodizing the surface of aluminum and aluminum alloys can produce various colors, providing both protection and decoration. It also creates an anodic oxide film on the material's surface, which has high hardness, wear resistance, electrical insulation, and thermal insulation properties.
4. Surface Brushing:
The material is placed between the upper and lower rollers of a brushing machine, with abrasive belts attached to the rollers. Driven by a motor, the material passes through the abrasive belts, leaving traces on its surface. The coarseness of the traces varies depending on the abrasive belt used. This method is mainly used for aesthetic enhancement and is commonly applied to aluminum materials.
5. Silk-Screen Printing:
This technique involves applying various markings on the material's surface. There are two main methods: flatbed screen printing and pad printing. Flatbed screen printing is mainly used on general flat surfaces, while pad printing is used for areas with deeper recesses.
