High-speed PCB design series basic knowledge 64 | PCB design post-processing DFM check

mwkjhl

High-speed PCB design series basic knowledge 64 | PCB design post-processing DFM check [Copy link]

This issue continues to introducethe post-processing methods of PCB design and what aspects are included in DFM inspection. 1. PCB width-to-thickness ratio requirement: Y/Z≤150 2. Transmission edge to non-transmission edge ratio requirement: 0.5≤X/Y≤5 If general reflow soldering tooling is required, at least one side of the PCB non-transmission edge should be designed with a device-free zone with a width of ≥5mm 3. When the PCB thickness is greater than 3mm, it is not recommended to use panel design or add auxiliary edge design. There are two main connection methods for panel and auxiliary edge, V-CUT and real connection. Only one connection method is allowed on a single board. V-CUT connection is preferred. V-CUT is a straight-through type. PCB thickness requirement for V-CUT design: 0.8mm≤board thickness≤3mm 4. V-CUT and PCB edge line or pad design requirements: [tr][td=97]

Safe distance

[/td][td=4,1,361]

s

[/td][/tr] [tr][td=97]

Plate thickness (mm)

[/td][td=87]

1.6

[/td][td=87]

[alig n=center]2

[/td][td=87]

2.5

[/td][td=98]

3

[/td][/tr] [tr][td=97]

Outer line (mm)

[/td][td=87]

0.6

[/td][td=87]

[alig n=center]0.7

[/td][td=87]

0.9

[/td][td=98]

1

[/td][/tr] [tr][td=97]

Inner line (mm)

[/td][td=87]

0.7

[/td][td=87]

0.8

[/td][td=87]

1

[/td][td=98]

1.1

[/td][/tr] [/table]

Requirements for V-CUT splitter to prohibit layout of components on half side of PCB

Device height h(mm)	Device forbidden area requirements (mm)
h(0--3)	≥1.0
h(3--5)	≥1.6
h(5-10)	≥2.0
h(10--13)	≥3.5
h(13--15)	≥4.0
h(15--33)	≥8.5
h(33--∞)	≥23

5.The distance requirements between stress sensitive devices (such as crystal oscillator of MLCC/BGA/ceramic substrate) and V-CUT connection are as follows:

Stress sensitive devices	Distance from V-CUT connection L (mm)
BGA device edge	L≥5
Ceramic capacitor 0402	L≥3
Ceramic capacitor 0603-0805	L≥5
Ceramic capacitor 1206-1210	L≥8
Ceramic capacitor 1808 and above	L≥10
Inductance 1812 and above	L≥4
Magnetic beads 1806 and above	L≥4
Crystal oscillator sx4-0705	L≥4

6. Real connection

Real connection is suitable for the connection of panels, complex panels, and auxiliary blocks with dense layouts.

Real connection design requirements forPCB:PCB size≤595mm*350mm,0.8mm≤board thickness≤4mm

Real connection extends outwardsComponents, traces, copper plating and vias are prohibited within the 0.5mm area

Positioning hole≥5mm from real connection edge

Stress sensitive device	Distance from real connection (mm)
BGA device edge	≥2
Ceramic capacitor C0805 and below	≥1
C1206 C1210	≥1.5
C1808 and above	≥2.5
Inductor 1812 and above	≥1
Magnetic beads 1806 and above	≥1
Crystal oscillator sx4-0705	≥1

7. Bend connectors are not recommended for use on the edge of V-CUT boards

Bend/male, bend/female crimping devices: On the same side as the crimping device, there shall be no components higher than 3mm around the crimping device, and there shall be no welding devices within 1.5mm around. On the reverse side of the crimping device, for crimping devices with a pin spacing of ≤4mm, there shall be no devices within 2.5mm from the center of the pin hole of the crimping device; for crimping devices with a pin spacing greater than 4mm, no devices shall be placed within a 2mm square range from the edge of the hole diameter.

8. Straight/male, straight/female crimping devices: There should be no devices within 1mm around the crimping device; when a sheath is required on the back of a straight/male, straight/female crimping device, no devices should be placed within 1mm from the edge of the sheath; when a sheath is not installed, no devices should be placed within 2.5mm from the center of the crimping hole.

9.Routing design

Line width/line spacing design is related to copper thickness. The thicker the copper, the larger the required line width/line spacing

Copper thickness	Outer layer line width/line spacing (mil)	Inner layer line width/line spacing (mil)
0.5Oz	4\5	4\4
1.0Oz	5\5	4\4
2.0Oz	7\7	6\6
3.0Oz	8\8	8\8

Distance between outer layer trace and pad or character solder mask opening≥3mil (hole edge to edge)

Distance from trace to board edge≥20milGround bus and ground copper foil are ≥20mil from board edge, distance from trace to non-metallized hole

[table] [tr][td=169]

Aperture

[/td][td=289]

Distance from trace to hole edge

[/td][/tr] [tr][td=169]

NPTH﹤80mil

[/td][td=289]

Stamp hole 40mil(the distance from the trace to the NPTH﹤80mil stamp hole is 40mil)

[/td][/tr] [tr][td=169]

[/td][td=289]

Mounting hole 20mil

[/td][/tr] [tr][td=169]

[/td][td=289]

Non-mounting hole 10mil

[/td][/tr] [tr][td=169]

80mil﹤NPTH﹤120mil

[/td][td=289]

Mounting hole 24mil

[/td][/tr] [tr][td=169]

[/td][td=289]

Non-mounting hole 12mil

[/td][/tr] [tr][td=169]

NPTH≥120mil

[/td][td=289]

Mounting hole 32mil

[/td][/tr] [tr][td=169]

Non-installation hole 16mil10. The gap between the cable heads should be ≥8mm so that you can hold the plug by hand to plug and unplug the cable. 11. Do not place the board name, LOGO, anti-static logo, etc. in the prohibited area for pin tin printing. 12. 0402, fine-pitch device pins are prohibited from copper plating. 13. Back drilling can reduce stubs and improve signal quality. HASL and LF-HASL are prohibited for PCB surface treatment with back drilling. 14. If the number of layers of plug-in connection exceeds 3, SMT devices are prohibited on the 6MM side that passes through wave soldering. 15. The thickness-to-diameter ratio of the board is between 8 and 12. If it exceeds, it depends on the manufacturer's processing capabilities. 16. THD device layout, except for special requirements of the structure, THD devices must be placed on the front, and the distance between adjacent component bodies ≧0.5mm

17. For SMDs that need to install heat sinks, attention should be paid to the installation position of the heat sink. The distance between the heat sink and the SMD device should meet the minimum installation space of 0.5mm

When the height of the heat sink is less than20mm, the distance from the edge of the board is greater than 10mm, and when it is higher than 20mm, the distance from the edge of the board is greater than 15mm (for the side of the handle, or when there are other protective structures on the edge of the single board, this restriction does not apply)

18. Secondary power supply

The pin height of the POL power module is 2.84mm, and the maximum height of the bottom side device is required to be less than 2.2mm; the pin boss height of the BMP power module is 3.5mm, and the maximum height of the bottom side device layout is required to be less than 3.0mm

19.Thick copper PCB stacking design

PCB recommends the use of Foil stacking method, with requirements of 0.8mm≤PCB board thickness≤3mm, recommended ≤3.0mm. The outer layer copper thickness is ≤2Oz, the inner layer bottom copper thickness is ≤5Oz, and the number of PCB layers is ≤12. When the copper thickness is ≥3Oz or the board thickness is ≥2.5mm, HASL surface treatment is prohibited

20. The distance between ordinary components on a single board and the edge of the transmission board must be greater than 5mm, and the distance between SOP\QFP\QFN\row resistors and capacitors, and 0402 resistors and capacitors and the edge of the transmission board must be greater than 10mm

21. Devices with metal shells (metal handles, horizontal voltage regulators, ferrite inductors, crystal oscillators and DPAK, guide pins, etc.) are not allowed to have routing in the area directly in contact with the PCB. Devices, signal lines and vias are prohibited from extending 1.5mm from the contact area between the metal shell of the device and the PCB. The surface of the connector with a metal shell is prohibited from wiring.

22. The 0402 device around the barcode is more than 10mm away from the barcode, and if a window is opened, it is more than 5mm

The above isDFM inspection for post-processing of PCB design.

This content is originally created by EEWORLD forum user mwkjhl. If you need to reprint or use it for commercial purposes, you must obtain the author's consent and indicate the source