Sheet metal bending refers to the processing of changing the angle of a sheet or panel.
For example, the plate is bent into a V shape, and U shape.
In general, there are two ways to bend a sheet metal:
One method is mold bending, which is used for sheet metal parts with complicated structures, small volume and large batch processing;
The other is press brake bending which is applied to the sheet metal structure with a relatively large structural size or a small yield.
These two bending methods have their own principles, characteristics and applicability.
Bending by mold
For structural parts with an annual processing capacity of more than 5,000 pieces and a part size not too large (generally 300X300), the processing manufacturer generally considers the mold bending.
Common bending mold
Commonly used bending dies, as shown in Figure 1-17: In order to extend the life of the mold, the parts should be designed with rounded corners.
Figure 1-17 Special Forming Mold
Too small a flange height, that is, the use of a bending die is also not conducive to forming, generally the height of the flange is L ≥ 3t (including the wall thickness).
Step bending method
Some of the lower-profile sheet metal Z-shaped steps are bent, and the processing manufacturers often use simple molds to machine on punch presses or hydraulic presses.
If the batch size is not large, it can be processed by the step die on the bending machine, as shown in Figure 1-18.
However, its height H cannot be too high and should generally be between (0～1.0) t.
If the height is (1.0～4.0) t, it is necessary to consider the mold form of the unloading structure according to the actual situation.
This mold step height can be adjusted by adding a spacer.
Therefore, the height H is arbitrarily adjusted.
However, there is also a disadvantage in that the length L size is not easily ensured, and the verticality of the vertical side is not easily ensured.
If the height H is large, consider bending on the press brake machine.
Figure 1-18 Z-shaped step bending
Bending by press brake machine
The bending machine is divided into two types: ordinary bending machine and CNC bending machine.
Due to the high precision requirements and the irregular shape of the bend, the sheet metal bending of the communication device is generally bent by a numerical control bending machine.
The basic principle is to bend and shape the sheet metal part by using the bending punch (upper mold) and the V-shaped die (lower mold) of the bending machine.
Convenient clamping, accurate positioning and fast processing speed;
The bending force is small, and it can only be processed by simple forming, and the efficiency is low.
Basic principles of forming
The basic principle of forming is shown in Figure 1-19:
Figure 1-19 Basic principle of forming
1) Bending knife (upper die)
The form of the bending knives is shown in Figure 1-20. The machining is mainly based on the shape of the workpiece.
Generally, the processing tool has a large number of bending knives.
In particular, the manufacturers with a high degree of specialization will custom-made bending knives of many shapes and specifications in order to process a variety of complex bending.
2) Lower die
The lower mold is generally V=6t (t is the material thickness).
There are many factors affecting the bending process, including the arc radius of the upper die, the material, the thickness of the material, the strength of the lower die, and the vee opening size of the lower die.
In order to meet the demand of the products, the manufacturer has already serialized the bending die in the case of ensuring the safety of the bending machine.
You need to have a general understanding of the existing bending die during the structural design process.
See Figure 1-20. The left side is the upper mold and the right side is the lower mold.
Figure 1-20 Schematic diagram of the press brake punch and die
The basic principle of the bending process sequence:
1) Bending from the inside to the outside;
2) Bending from small to large;
3) Bend the special shape first and then bend the general shape;
4) After the previous process is formed, it does not affect or interfere with the subsequent process.
The bending forms seen by the current outsourcing factory are generally shown in Figure 1-21.
Figure 1-21 Bending form of press brake machine
When the sheet metal is bent, a bend radius is required at the bend.
The bending radius should not be too large or too small and should be chosen appropriately.
If the bending radius is too small, the bending will be cracked, and if the bending radius is too large, the bending is easy to rebound.
The preferred bending radius (inside bending radius) of various materials with different thicknesses is shown in Table 1-9 below.
|Material||Annealed state||Cold work hardening state|
|The corresponding position of the direction of the bending line and the direction of the fiber|
|08,10||0.1t||0.4 t||0.4 t||0.8 t|
|15,20||0.1 t||0.5 t||0.5 t||1.0 t|
|25,30||0.2 t||0.6 t||0.6 t||1.2 t|
|45,50||0.5 t||1.0 t||1.0 t||1.7 t|
|65Mn||1.0 t||2.0 t||2.0 t||3.0 t|
|Aluminum||0.1 t||0.35 t||0.5 t||1.0 t|
|Copper||0.1 t||0.35 t||1.0 t||2.0 t|
|Soft brass||0.1 t||0.35 t||0.35 t||0.8 t|
|Semi-hard brass||0.1 t||0.35 t||0.5 t||1.2 t|
|Phosphor bronze||——||——||1.0 t||3.0 t|
Note: t is the thickness of the sheet in the table.
The data in the above table is the preferred data and is for reference only.
In fact, the manufacturer’s bending knives usually have a rounded corner of 0.3, and a small number of bending knives have a rounded corner of 0.5.
Therefore, the bending inner radius of our sheet metal parts is basically 0.2.
For ordinary low-carbon steel plates, rust-proof aluminum plates, brass plates, copper plates, etc., the inner radius of 0.2 is no problem.
However, for some high-carbon steel, hard aluminum, and super-hard aluminum, this rounded corner will cause the bend to break or the outer corner to crack.
Figure 1-22 Bending and rebounding diagram
1) Rebound angle Δα=b-a
In the formula:
- b – the actual angle of the workpiece after the rebound;
- a – the angle of the mold.
2) The size of the rebound angle
The rebound angle at 90° air bend is shown in Table 1-10.
Table 1-10 Rebound angle at 90-degree air bend
|Medium carbon steel σb=400-500MPa||<1||5°||2°||0°|
|Hard yellow copper σb=350-400MPa||1~5||6°||3°||1°|
|Hard bronze σb=350-400MPa||>5||8°||5°||3°|
|High carbon steel σb>550Mpa||<1||7°||4°||2°|
- Factors affecting rebound and measures to reduce rebound.
- Mechanical properties of the material
The size of the rebound angle is proportional to the yield point of the material and inversely proportional to the elastic modulus E.
For sheet metal parts with high precision requirements, in order to reduce the rebound, the material should be as low-carbon steel as possible, not high-carbon steel and stainless steel.
- The larger the relative bending radius r/t, the smaller the degree of deformation, and the larger the rebound angle Δα.
This is a more important concept.
The rounded corners of sheet metal bends should be selected with a small bend radius as much as possible, which is beneficial to improve accuracy.
In particular, it should be avoided to design large arcs as much as possible, as shown in Figure 1-23.
Such large arcs are more difficult for production and quality control.
Figure 1-23 The arc of the sheet metal is too large
Calculation of the minimum bend edge of a bend
The initial state of the bend of the L-shaped bend is shown in Figure 1-24:
Figure 1-24 L-bend bending
One important parameter here is the width B of the lower die.
Due to the bending effect and the strength of the mold, there is a minimum width of the die required for materials of different thicknesses.
When it is less than this value, there will be a problem that the bending is not in place or the mold is damaged.
It has been proved by practice that the relationship between the minimum die width and the material thickness is:
Bmin = kT ①
Bmin is the minimum mold width, T is the material thickness, and K=6 when calculating the minimum die width.
At present, the specifications of the bending die width commonly used by manufacturers are as follows:
4, 5, 6, 8, 10, 12, 14, 16, 18, 20, 25
According to the above relationship, the minimum thickness of the lower die width required for different material thicknesses during bending can be determined.
For example, when a 1.5mm thick plate is bent, B=6*1.5=9. For the die width series above, you can choose a die width of 10mm (or 8mm) of the lower die.
From the initial state diagram of the bend, it can be seen that the edge of the bend cannot be too short.
Combined with the minimum die width above, the formula for obtaining the shortest bend edge is ②: (see Figure 1-25)
Lmin is the shortest bent edge, Bmin is the minimum die width, and Δ is the bending coefficient of the sheet.
When the 1.5mm thick plate is bent, the shortest bend edge Lmin = (8 + 2.5) / 2+0.5 = 5.75mm (including a plate thickness).
Figure 1-25 Minimum die width
Table 1-11: Inner bending radius of cold rolled steel sheet material R and minimum bending height reference table
|No.||Thickness||V opening||Punch radius R||Min bending height|
|3||0.8||5||0.8 or 0.2||3.7|
|4||1||6||1 or 0.2||4.4|
|5||1.2||8（or 6）||1 or 0.2||5.5（or 4.5）|
|6||1.5||10（or 8）||1 or 0.2||6.8（or 5.8）|
|7||2||12||1.5 or 0.5||8.3|
|8||2.5||16（or 14）||1.5 or 0.5||10.7（or 9.7）|
|9||3||18||2 or 0.5||12.1|
- The minimum bend height contains a material thickness.
- When the V-bend is an acute angle, the shortest bend must be increased by 0.5.
- When the part material is aluminum plate and stainless steel plate, the minimum bending height will have small changes. The aluminum plate will become smaller, the stainless steel will be larger, refer to the above table….
Minimum bend height for Z-bends
The initial state of the Z-bend bend is shown in Figure 1-26:
The Z-bend and L-bend processes are very similar, and there is also a minimum bend edge problem.
Due to the structure of the lower die, the shortest edge of the Z-bend is larger than the L-bend.
The formula for calculating the minimum edge of a Z-bend is:
Lmin=1/2(Bmin+Δ)+D + 0.5 + T ③
Lmin is the shortest bend edge, Bmin is the minimum mold width, Δ is the bending coefficient of the sheet, T is the material thickness, and D is the structural size of the lower die to the edge, generally greater than 5mm.
Figure 1-26 Z-bend
The minimum bend size L for sheet metal Z-bends of different material thicknesses is shown in Table 1-12 below:
Table 1-12 Minimum height of Z bend
|No||Thickness||V opening||Punch radius R||Z -bend height L|
|3||0.8||5||0.8 or 0.2||9.5|
|4||1||6||1 or 0.2||10.4|
|5||1.2||8（or 6）||1 or 0.2||11.7（or 10.7）|
|6||1.5||10（or 8）||1 or 0.2||13.3（or 12.3）|
|7||2||12||1.5 or 0.5||14.3|
|8||2.5||16（or 14）||1.5 or 0.5||18.2（or 17.2）|
|9||3||18||2 or 0.5||20.1|
Interference during bending
For secondary or above secondary bending, it is often the case that the bending workpiece interferes with the tool.
As shown in Figure 1-27, the black part is the interference part, so the bending cannot be completed, or the bending deformation is caused by the bending interference.
Figure 1-27 Interference of bending
The interference problem of sheet metal bending does not involve too much technology.
Just understand the shape and size of the bending die, and avoid the bending die when designing the structure.
Figure 1-28 shows the cross-sectional shapes of several common bending knives, which are described in the sheet metal mold manual, and there are corresponding tool entities in the intralink library.
In the case of unsure design, the assembly interference test can be directly performed with the tool according to the principle of the above figure.
Figure 1-28 Bending knife
For flip hole tapping, the D value shown in Figure 1-29 cannot be designed too small.
The minimum D value can be calculated or plotted based on material thickness, through hole outer diameter, flange hole height, and selected bending tool parameters.
For example, a flip hole tapping of an M4 with a 1.5 mm sheet bent, the D value should be greater than 8 mm. Otherwise, the bending knife will hit the flange.
Figure 1-29 Bending of the hole flanging & tapping
Minimum distance between the hole and the oblong hole
As shown in Figure 1-30, the edge of the hole at the bend is too close to the fold line. When the bend is performed, it cannot be taken up, resulting in a change in the shape of the hole.
Therefore, the hole edge and the bend line are required to be larger than the minimum hole margin X ≥ t + R.
Figure 1-30 Minimum distance from the round hole to the bent edge
Table 1-13 Minimum distance from the round hole to the bent edge
|Min Distance X||1.3||1.5||1.7||2||3||3.5|
As shown in Figure 1-31, the oblong hole is too close to the fold line.
When the bend is performed, the material cannot be taken up, and the shape of the hole is deformed.
Therefore, the hole edge and the bend line are required to be larger than the minimum hole margin (refer to table 1-14), and the bend radius refers to Table 1-9.
Figure 1-31 The minimum distance from the long round hole to the bent edge
Table 1-14 Minimum distance from the long round hole to the bent edge
|Min distance X||2t+R||2.5t+R||3t+R|
For unimportant holes, expand the hole to the bend line, as shown in Figure 1-32.
Disadvantages: affect the appearance.
Figure 1-32 Improved bending design
Special processing when the hole is close to the bend
When the distance from the hole which closes to the bend line to the bent edge is less than the minimum distance described above, deformation will occur after the bend.
At this time, according to the different requirements of the product, it can be handled as shown in the following Table 1-15.
However, it can be seen that the technicality of these methods is poor, and the structural design should be avoided as much as possible.
Table 1-15 Special processing when the hole is close to the bend
1) Press the groove before bending.
In the actual design, because of the structural design needs, the actual distance is smaller than the above distance.
The processing manufacturer often performs the groove pressing before the bending, as shown in Figure 1-31.
The disadvantage is: one extra process is needed for the bending processing, the efficiency is lower, the precision is lower, and in principle, it should be avoided as much as possible.
2) Cut hole or line along the bend line: when the bend line has no effect on the appearance of the workpiece or is acceptable, then use hole cutting to improve its techniques.
Disadvantages: affect the appearance. And when cutting a line or cutting a narrow groove, it is generally necessary to cut with a laser machine.
3) Completion to the design size after bending at the edge of the hole near the bend line.
When the hole margin is required, it can be handled in this way.
Generally, this secondary material removal cannot be completed on a punching machine, and the second cutting can only be performed on the laser cutting machine, and the positioning is troublesome, and the processing cost is high.
4) After the bending, the hole reaming process only has one or several pixel holes to the bending line and the distance is less than the minimum hole distance.
When the appearance of the product is strict, in order to avoid the drawing during bending, the pixel can be performed at this time.
Shrinkage treatment, that is, cutting a small concentric circle (usually Φ1.0) before bending, and reaming to the original size after bending.Disadvantages: many projects, low efficiency.
5) The minimum width of the upper die of the bending machine is 4.0mm (current).
Due to this limitation, the hole in the bending part of the workpiece shall not be less than 4.0mm.
Otherwise, the opening must be enlarged or use easy to form die to perform the bending.
Disadvantages: low efficiency in making the easy mold, low efficiency in easy mold production; reaming affects appearance.
Process holes, process slots and process notches for curved parts
When designing the bending part, if the bending part has to bend the bending edge to the inner side of the blank, the punching process hole, process groove or process notch should generally be added before blanking, as shown in Figure 1-33.
Figure 1-33 Adding punch hole, process or process notch
D- diameter of the process hole, d ≥ t;
K-process notch width, K ≥ t.
Crack avoid groove or cut slit:
In general, for a part of an edge to bend, in order to avoid tearing and distortion, the crack avoid groove or cut slit should be opened.
Especially for bending with an inner corner of fewer than 60 degrees, it is necessary to open the crack groove or the slit.
The width of the slit is generally greater than the thickness t, and the depth of the slit is generally greater than 1.5t.
In figure 1-34, Figure b is more reasonable than Figure a.
Figure 1-34 Bending of the sheet with the crack groove or slit
The process groove and process hole should be processed correctly, and if the workpieces can be seen from the panel and the appearance, then the cornering process holes of the bending can be not added (for example, the process notch is not added in the process of planel processing in order to maintain a uniform style), and other bends should add the cornering process hole, as shown in Figure 1-35.
Figure 1-35 Bending corner process hole
When designing the drawings, if there is no special requirement, do not mark the gap between the bending collisions in the 90 ° direction.
Some unreasonable gap markings affect the process design of the manufacturer.
The processing manufacturer generally designs the process according to the gap of 0.2 to 0.3. As shown in Figure 1-36:
Figure 1-36 the gap between the bend lapping
Bending of a sudden change position
The bending zone of the bending part should avoid the location of the sudden change of the part.
The distance L of the bending line from the deformation zone should be greater than the bending radius r, ie L≥r, as shown in Figure 1-37
Figure 1-37 The bend zone should avoid the location of the sudden change of the part
One time hemming
The way for hemming: As shown in Figure 1-38, first fold the sheet to 30 degrees with a 30-degree bending knife, and then flatten the bent side.
Figure 1-38 Method of hemming
The minimum bend edge dimension L in the figure is 0.5t (t is the material thickness) according to the minimum bend edge size of the one-bend edge described above.
The pressed dead edge is generally applied to stainless steel, galvanized sheet, and aluminum-zinc plate.
Plating parts should not be used, because there is a phenomenon of acid trapping in the place where the hemming is performed.
180-degree bend method:
As shown in Figure 1-39, first fold the plate to 30 degrees with a 30-degree bending knife, then flatten the bending edge, and then pull out the pad.
Figure 1-39 180-degree bend method
The minimum bend edge dimension L in the figure is the minimum bend edge dimension of one bend edge plus t (t is the material thickness), and the height H should be selected from commonly used plates, such as 0.5, 0.8, 1.0, 1.2, 1.5, 2.0.
Generally, this height is not suitable for selecting a higher size.
Triple folding hemming
As shown in Figure 1-40, fold the shape first, then fold the edge.
Pay attention to the dimensions of each part during design to ensure that each processing step meets the minimum bending size and avoid unnecessary post-processing.
Figure 1-40 Triple folding hemming
Table 1-16 Minimum bearing edge size required for final bending edge flattening
|Bearing edge size L||4.0||4.0||4.0||4.0||4.5||4.5||5.0||5.0|