Sheet Metal Design Tips and How to Optimize It

Preface

Sheet metal parts are widely used in automobile surface covering parts and internal structural parts.

My main business is controller structural engineer, and I always bear the pressure of cost reduction.

After investigating various schemes, I found that the peers had successfully changed the upper cover of the controller into a sheet metal stamping part.

In order to avoid making low-level mistakes in the design process, I consulted the data and displayed the common skills of sheet metal part design here, and hope to communicate and learn with all friends in the same industry.

Sheet Metal Design Tips and How to Optimize It 1

There are four major processes in sheet metal processing: blanking, bending, stretching and forming.

Each process has its own specification requirements on design, and we will briefly describe them from these four aspects.

1. Blanking

Blanking is divided into ordinary blanking and precision blanking.

Due to different processing methods, the processing technology of blanking parts is also different.

The upper cover of the motor controller and other structural parts are generally only used for ordinary blanking.

The following will only introduce the structure and technology of common blanking that we can use.

Skill 1.1

The shape and size of blanking parts shall be as simple and symmetrical as possible to minimize waste during layout.

Sheet Metal Design Tips and How to Optimize It 2

Layout of blanking parts

Skill 1.2

Sharp corners shall be avoided in the shape and inner hole of blanking parts.

Arc connection shall be provided at the connection of straight line or curve, with arc radius R ≥ 0.5t. (t is material wall thickness)

Sheet Metal Design Tips and How to Optimize It 3

Minimum value of fillet radius of blanking part

Skill 1.3

The depth and width of the convex or concave part of the blanking parts with narrow cantilever and slot shall be avoided.

Generally, it shall not be less than 1.5t (t is the material thickness).

Meanwhile, narrow and long notches and excessively narrow notches shall be avoided to increase the edge strength of the corresponding parts of the die.

Sheet Metal Design Tips and How to Optimize It 4

Avoid narrow cantilevers and grooves.

Skill 1.4

Circular holes are preferred for punching, and circular holes are preferred for punching with minimum size requirements.

The minimum size of punching is related to the shape of the hole, the mechanical properties of the material and the thickness of the material.

Sheet Metal Design Tips and How to Optimize It 5

Punch shape example

MaterialDiameter of circular hole (b)Width b of short side of rectangular hole
High-carbon steel1.3t 1.0t
Low carbon steel, brass1.0t0.7t
Aluminium0.8t0.5t

*t is the material thickness, and the minimum size of punching is generally not less than 0.3mm

Skill 1.5

Punching hole spacing and hole edge spacing.

The minimum distance between the punching edge of the part and the shape is limited according to the shape of the part and the hole, as shown in the following figure.

When the punching edge is not parallel to the outline edge of the part, the minimum distance shall not be less than the material thickness t; When parallel, it shall not be less than 1.5t.

Sheet Metal Design Tips and How to Optimize It 6

Schematic diagram of hole edge distance and hole spacing of blanking parts

Skill 1.6

When punching bending parts and drawing parts, a certain distance shall be kept between the hole wall and the straight wall.

Sheet Metal Design Tips and How to Optimize It 7

Distance between the hole wall of the bending part and the stretching part and the straight wall of the workpiece

Skill 1.7

Through holes and countersunk seats for screws and bolts.

The structural dimensions of screw, bolt through hole and countersunk head seat are selected in the following table.

For the countersunk head seat of countersunk head screw, if the plate is too thin to guarantee the through hole d2 and the countersunk hole D at the same time, the through hole d2 shall be ensured preferentially.

Sheet Metal Design Tips and How to Optimize It 8

d1

M2

M2.5

M3

M4

M5

M6

M8

M10

d2

Φ2.2

Φ2.8

Φ3.5

Φ4.5

Φ5.5

Φ6.5

Φ9.0

Φ11

Through holes for screws and bolts

Sheet Metal Design Tips and How to Optimize It 9

d1

M2

M2.5

M3

M4

M5

d2

Φ2.2

Φ2.8

Φ3.5

Φ4.5

Φ5.5

D

Φ4.0

Φ5.5

Φ6.5

Φ9.0

Φ10.

h

1.2

1.5

1.65

2.7

2.7

a

90°

*It is required that the sheet metal thickness t ≥ h.

Countersunk head seat and through hole for countersunk head screws

Sheet Metal Design Tips and How to Optimize It 10

d1

Φ2

Φ2.5

Φ3

Φ4

Φ5

d2

Φ2.1

Φ2.6

Φ3.1

Φ4.1

Φ5.1

D

Φ4.1

Φ5

Φ5.5

Φ7.2

Φ9

h

1

1.1

1.2

1.6

2

a

90°

*It is required that the sheet metal thickness t ≥ h.

Countersunk seat and through hole for countersunk rivet

Skill 1.8

The limit value of the burr of the blanking part and the design mark that the burr of the blanking part exceeds a certain height are not allowed.

The limit value (mm) of the burr height of the stamping part is shown in the following table.

Material wall thickness

Material tensile strength (N / mm2)

>100~250

>250~400

>400~630

>630

f

m

g

f

m

g

f

m

g

f

m

g

>0.7~1.0

0.12

0.17

0.23

0.09

0.13

0.17

0.05

0.07

0.1

0.03

0.04

0.05

>1.0~1.6

0.17

0.25

0.34

0.12

0.18

0.24

0.07

0.11

0.15

0.04

0.06

0.08

>1.6~2.5

0.25

0.37

0.5

0.18

0.26

0.35

0.11

0.16

0.22

0.06

0.09

0.12

>2.5~4.0

0.36

0.54

0.72

0.25

0.37

0.5

0.2

0.3

0.4

0.09

0.13

0.18

*Grade f (precision grade) is applicable to parts with higher requirements;

m level (medium level) is applicable to parts with medium requirements;

Grade g (roughness) is applicable to parts with general requirements.

2. Bending

Skill 2.1

The minimum bending radius of the bending part: when the material is bent, the outer layer is stretched and the inner layer is compressed in the fillet area.

When the thickness of the material is constant, the smaller the internal R, the more serious the tension and compression of the material;

When the tensile stress of the outer fillet exceeds the ultimate strength of the material, cracks and fractures will occur.

Therefore, the structural design of the bending parts should avoid too small bending fillet radius.

The minimum bending radius of common materials of the company is shown in the following table.

Serial number:MaterialMinimum bending radius
108, 08F, 10, 10F, DX2, SPCC, E1-T52, 0Cr18Ni9, 1Cr18Ni9, 1Cr18Ni9Ti, 1100-H24, T20.4t
215, 20, Q235, Q235A, 15F0.5t
325, 30, Q2550.6t
41Cr13, H62 (M, Y, Y2, cold rolling)0.8t
545, 501.0t
655, 601.5t
765Mn, 60SiMn, 1Cr17Ni7, 1Cr17Ni7-Y, 1Cr17Ni7-DY, SUS301, 0Cr18Ni9, SUS3022.0t

The bending radius refers to the inner radius of the bending part, and t is the wall thickness of the material.

t is the wall thickness of the material, M is the annealed state, Y is the hard state, and Y2 is the 1 / 2 hard state.

List of minimum bending radius of common metal materials

Skill 2.2

The height of the straight edge of the bent part should not be too small.

The minimum height is as follows: h > 2t.

Sheet Metal Design Tips and How to Optimize It 11

The minimum value of the straight edge height of the bending part:

If the design requires the straight edge height of the bending part h ≤ 2t, the bending height shall be increased first, and then processed to the required size after bending;

Or after processing the shallow groove in the bending deformation area, bend it again (as shown in the figure below).

Sheet Metal Design Tips and How to Optimize It 12

The height of straight edge in special cases requires the height of straight edge with oblique angle on the side of the bend.

When the side of the bending part is provided with an oblique angle (as shown in the figure below), the minimum height of the side is: h = (2-4) t > 3mm.

Sheet Metal Design Tips and How to Optimize It 13

Height of straight edge with beveled edge

Skill 2.3

Hole edge distance on bent parts hole edge distance:

The hole shall be punched first and then bent.

The position of the hole shall be outside the bending deformation area to avoid deformation of the hole during bending.

See the table below for the distance from the hole wall to the bending edge.

Sheet Metal Design Tips and How to Optimize It 14

Sheet Metal Design Tips and How to Optimize It 15

t(mm)

s(mm)

1(Mm)

s(mm)

≤25

s≥2t+r

≤2.

s≥t+r

>25~50

s≥2.5t+r

>2

s≥1.5t+r

>50

s≥3t+r

Height of straight edge with beveled edge

Skill 2.4

When a section of edge is locally bent by a locally bent process notch, in order to prevent bending crack caused by stress concentration at the sharp corner, the bending curve can be moved a certain distance to leave the sudden change of size (Fig. a), or the process groove (Fig. b) or the process hole (Fig. c) can be punched.

Note the dimensional requirements in the drawing: s ≥ R; Groove width K ≥ t; Groove depth L ≥ t + R + K / 2.

Sheet Metal Design Tips and How to Optimize It 16

Design and processing method of local bending when the hole is in the bending deformation area, the example of notch form is adopted.

Sheet Metal Design Tips and How to Optimize It 17

Example of notch form

Skill 2.5

The bending edge with beveled edge shall avoid the deformation area.

Sheet Metal Design Tips and How to Optimize It 18

The bending edge with beveled edge shall avoid the deformation area.

Skill 2.6

The design of the dead edge requires that the dead edge length of the dead edge is related to the thickness of the material.

As shown in the figure below, the minimum length L of dead edge is generally ≥ 3.5t + R.

Where t is the wall thickness of the material, and R is the minimum inner bending radius of the previous process (as shown in the right figure below) before the edge is killed.

Sheet Metal Design Tips and How to Optimize It 19

Minimum length of dead edge (L)

Skill 2.7

Process positioning holes added in the design to ensure the accurate positioning of the blank in the mold and prevent waste products caused by the deviation of the blank during bending, process positioning holes shall be added in the design in advance, as shown in the following figure.

Especially for the parts formed by multiple bending, the process hole must be used as the positioning reference to reduce the accumulated error and ensure the product quality.

Sheet Metal Design Tips and How to Optimize It 20

Process positioning holes added during multiple bending

Skill 2.8

When marking the relevant dimensions of bent parts, the process shall be considered.

Sheet Metal Design Tips and How to Optimize It 21

For example, as shown in the above figure,

a) Punching first and then bending, L-dimension accuracy is easy to ensure and processing is convenient.

b) And c) if the accuracy of dimension L is required to be high, it needs to be bent before machining holes, which is troublesome.

Skill 2.9

There are many factors that affect the springback of bending parts, including the mechanical properties of materials, wall thickness, bending radius and positive pressure during bending.

The larger the ratio of the inner radius of the bent part to the plate thickness, the greater the springback.

The springback of bending parts is an example of the method to suppress springback from the design.

At present, the manufacturer mainly takes certain measures to avoid the springback in the mold design.

At the same time, some structures are improved from the design to make the springback angle simple as shown in the following figure: pressing the reinforcing rib in the bending area can not only improve the rigidity of the workpiece, but also help to suppress the springback.

Sheet Metal Design Tips and How to Optimize It 22

Examples of methods for suppressing springback in design

3. Stretching

Skill 3.1

The fillet radius between the bottom of the stretching part and the straight wall shall be as shown in the following figure.

The fillet radius between the bottom of the stretching part and the straight wall shall be greater than the plate thickness, i.e. r1 ≥ t.

In order to make the stretching more smoothly, r1 = (3 ~ 5) t is generally taken, and the maximum fillet radius should be less than or equal to 8 times of the plate thickness, i.e. r1 ≤ 8t.

Sheet Metal Design Tips and How to Optimize It 23

Example of bend dimension

Skill 3.2

The fillet radius between the flange and the wall of the stretching piece the fillet radius between the flange and the wall of the stretching piece shall be greater than 2 times of the plate thickness, i.e. r2 ≥ 2t.

In order to make the stretching more smoothly, generally r2 = (5 ~ 10) t is taken, and the maximum flange radius shall be less than or equal to 8 times of the plate thickness, i.e. r2 ≤ 8t.

(see figure above)

Skill 3.3

The diameter of the inner cavity of the circular stretching piece the diameter of the inner cavity of the circular stretching piece shall be taken as d ≥ d + 10t, so that the pressing plate will not wrinkle during stretching. (see figure above)

Skill 3.4

Fillet radius between adjacent two walls of rectangular stretching piece the fillet radius between adjacent two walls of rectangular stretching piece shall be r3 ≥ 3t.

In order to reduce the stretching times, r3 ≥ H / 5 shall be taken as much as possible so as to pull out at one time.

Sheet Metal Design Tips and How to Optimize It 24

Fillet radius between two adjacent walls of rectangular stretching part

Skill 3.5

The ratio of height h to diameter d shall be less than or equal to 0.4, i.e. H / d ≤ 0.4, as shown in the figure below, when the circular flangeless tensile part is formed at one time.

Sheet Metal Design Tips and How to Optimize It 25

Dimensional relationship between height and diameter of circular flangeless stretch parts during one-time forming

Skill 3.6

Precautions for dimension marking on the design drawing of tensile parts: the tensile parts are subject to different stress levels, resulting in changes in the material thickness after stretching.

Generally speaking, the center of the bottom keeps the original thickness, the material at the bottom corner becomes thinner, the material at the top near the flange becomes thicker, and the material at the corner around the rectangular stretching part becomes thicker.

1. When designing tensile products, the dimensions on the product drawing shall be clearly indicated that the external or internal dimensions must be guaranteed, and the internal and external dimensions cannot be marked at the same time.

2. The inner radius of the concave convex arc of the stretching part and the height dimension tolerance of the cylindrical stretching part formed at one time are double-sided symmetrical deviations, and the deviation value is half of the absolute value of the accuracy tolerance of grade 16 of the national standard (GB), and is marked with ± sign.

4. Forming

Skill 4.1

Pressing ribs on plate-shaped metal parts helps to increase the structural rigidity.

See the following figure for the structure and size selection of reinforcing ribs.

NamediagramRhB or Drα °
StiffenSheet Metal Design Tips and How to Optimize It 26 (3~4)t(3~2)t(7-10)t(1~2)t
ConvexSheet Metal Design Tips and How to Optimize It 27 (2~1.5)t≥3h(0.5~1.5)t15~30

Structure and size selection of stiffeners

Skill 4.2

The limit dimensions of convex spacing and convex edge spacing are selected in the following table.

Diagram

D

L

1

Sheet Metal Design Tips and How to Optimize It 28

6.5

10

6

8.5

13

7.5

10.5

15

9

13

18

11

15

22

13

18

26

16

24

34

20

31

44

26

36

51

30

43

60

35

48

68

40

55

78

45

Structure of louvers

Size requirements of louvers: a ≥ 4t; b≥6t; h≤5t; L≥24t; r≥0.5t.

Skill 4.3

Louvers are usually used on various covers or casings for ventilation and heat dissipation.

The forming method is to cut the material by one edge of the punch, and the rest of the punch will stretch and deform the material at the same time to form an undulating shape with an opening on one side.

The typical structure of louvers is shown in the following figure.

Sheet Metal Design Tips and How to Optimize It 29

Structural louver size requirements: a ≥ 4t; b≥6t; h≤5t; L≥24t; r≥0.5t.

Skill 4.4

Internal hole flanging of machining thread

Sheet Metal Design Tips and How to Optimize It 30

Schematic diagram of internal hole flanging structure with threaded hole

screw thread

Material thickness (t)

Flanging inner hole D1

Flanging outer hole d2

Flange height (h)

Pre punching diameter D0

Flange fillet radius R

M3

0.8

3.38

1.6

1.9

0.6

3.25

1.6

2.2

1

3.38

1.8

1.9

0.5

2.55

3.5

2

2

1.2

3.38

1.92

2

0.6

3.5

2.16

1.5

1.5

3.5

2.4

1.7

0.75

M4

1

4.46

2

2.3

0.5

4.35

1.92

2.7

1.2

4.5

2.16

2.3

0.6

3.35

4.65

2.4

1.5

1.5

4.46

2.4

2.5

0.75

4.65

2.7

1.8

2

4.56

2.2

2.4

1

1.2

5.6

2.4

3

0.6

M5

5.46

2.4

2.5

1.5

5.6

2.7

3

0.75

4.25

5.75

3

2.5

2

5.53

3.2

2.4

5.75

3.6

2.7

1

2.5

5.75

4

3.1

1.25

1.5

7

3

3.6

0.75

6.7

3.2

4.2

M6

2

7

3.6

3.6

1

5.1

7.3

4

2.5

2.5

7

4

2.8

7.3

4.5

3

1.25

3

7

4.8

3.4

1.5

Internal hole flanging dimension parameters with threaded holes

5. How to optimize sheet metal design?

Sheet Metal Design Tips and How to Optimize It 31

Generally, sheet metal processing is the process of cold processing with metal sheet to obtain sheet metal parts that meet the application requirements.

Generally, sheet metal parts have obvious advantages such as strength, weight and cost, and have better performance than traditional parts.

Therefore, up to now, sheet metal parts have been gradually applied in high-tech fields such as electronics and communications in China,

At the same time, people have gradually put forward higher requirements for the quality and function of sheet metal parts.

Therefore, appropriate optimization of the original sheet metal processing technology has become the focus of sheet metal processing personnel.

According to the actual research, this paper thinks that the optimization of the processing technology should be carried out one by one from the application of the four basic cold processing links in the sheet metal processing.

1. Blanking

First of all, as far as the blanking link is concerned, generally speaking, blanking refers to the separation of sheet metal materials from each other through the punching of the die, so as to realize the separation of sheet metal.

This link is usually used in the processing of parts with relatively simple shape, so as to achieve a high degree of accuracy of the processing shape and minimize the waste of materials.

At this stage, firstly, the shape of blanking sheet metal parts should be controlled.

In the corner area of the outer and inner holes of blanking, the arc should be set to reduce the excessive angle, avoid the sharp angle and reduce the mold cracking caused by improper subsequent heat treatment, which will affect the subsequent sheet metal construction;

Then, the punching and its minimum value should be optimized.

In general, when punching sheet metal parts, if the punching size of the punched sheet metal parts is small, the load on the punch will be greatly reduced.

However, if it is too small, it is easy to cause the data of the pressure borne by the die to become more suddenly, and then affect the quality of the actual die.

For example, in this stage, the punching of sheet metal parts should be set according to different load targets of sheet metal parts.

In the basic state, the length of the hole should be more than twice the hole spacing and more than 3.00mm.

Finally, the cantilever and groove setting on the blanking part should be avoided from being too narrow or too long in the actual process application, so as to improve the strength of the relevant die edge and control the cantilever notch width to be greater than 200 metal plate thickness.

Sheet Metal Design Tips and How to Optimize It 32

2. Bending

Generally, the bending link refers to the process of preventing and curing sheet metal materials on the bending equipment, causing elastic deformation of sheet metal materials through the pressure of the upper die or the lower die, and plastic deformation according to the actual design scheme after elastic deformation.

In the application process of this link, different parts should be selected according to the actual design requirements, and the actual operation of bending should be determined according to the thickness of sheet metal raw materials.

According to the actual bending experience, local abnormal deformation is most likely to occur in the bending process, which will affect the appearance quality and actual application of sheet metal parts.

Therefore, in the actual operation, if you want to optimize the bending process, the operator should make a cut in advance according to the actual situation, so as to avoid the subsequent deformation.

At the same time, when the parts need to be bent for many times, a comprehensive prediction should be made in all the bending operation links to avoid the previous bending operation affecting the subsequent bending process, so as to achieve the expected design goal of sheet metal parts.

3. Press riveting

Sheet Metal Design Tips and How to Optimize It 33

The press riveting process of sheet metal parts refers to the process of deforming sheet metal materials through the action of pressure and coupling them together.

This process is usually applied to screw press riveting, bolt press riveting and other processes.

As for the end press riveting operation process, the nut usually presents a circular shape and a section of embossed gear and wire slot.

Therefore, the riveting process of sheet metal parts not only optimizes the quality of the original nut manufacturing process, but also avoids the welding work.

If you want to obtain a better design scheme, first of all, you can select different specifications of molds according to the height of different pressed bolts in the actual press riveting process, and adjust the pressure release of the press riveting device to ensure the nut pressing quality and avoid the problem of waste parts.

Secondly, the appropriate sheet metal size can be selected in the setting of the press riveting structure, so as to ensure the press riveting results and avoid the release of the press link of the sheet metal parts.

4. Welding

Sheet Metal Design Tips and How to Optimize It 34

Welding is one of the important ways to connect the structures of all parts in the cold working process of the whole sheet metal processing process.

Therefore, this process is usually placed under the high temperature background for operation.

At present, most of the common welding methods are argon arc welding and contact spot welding.

Therefore, in the actual welding process, different welding methods should be selected according to the properties of different sheet metal parts, so as to minimize the welding deformation and improve the actual welding efficiency.

For example, in the actual welding process, first of all, sufficient welding control shall be determined.

Secondly, the length of the welding part shall be controlled accurately to avoid the deformation of the sheet metal and optimize the load of the welding point.

Leave a Comment

Your email address will not be published.

Scroll to Top