1. General

(1) When the design rules are satisfied, the production cost should be reduced as much as possible, for example, if the two-layer board can be used, try to use the two-layer board; when the cost conflicts with the design rules, the design rules should be guaranteed.

(2) The components are arranged neatly, and the same chips are arranged in rows and columns according to certain rules; the spacing of components should consider the production process and cannot affect the welding.

(3) For PCB design, automatic routing cannot be used for design.

2. Details

(1) Use of wiring layer

When designing a circuit board with more than 2 layers, it is forbidden to use the inner electric layer. Use inner layer definitions like normal layers.

For cell boards that require blind via buried via design, for four-layer boards, punch holes 1-2, 3-4, 1-4; for six-layer boards, punch holes 1-2, 2-5, 5-6; specific The process must be confirmed with the PCB manufacturer after confirmation.

(2) Separate power supply for digital devices and driving devices

To adopt the method of separate wiring of digital ground and analog ground, the power supply of the digital part is only connected to the power supply of the driving part through a jumper at the entrance of the power socket.

In the case of space on the board, it is recommended to separate the power supply for the column drive and the power supply for the row drive as well.

(3) Power cord and line:

The power rail width of the digital part is >=50mil.

The width of the power lines and row lines should comprehensively consider the current, width, and distance of the power branch. Ensure that the voltage drop on the line from the power inlet to the module is not greater than 0.01V.

It is recommended that the power socket be placed in the middle of the board. When the power socket is placed on one side, reserve power sockets or pads on the symmetrical side to facilitate flying wires during production.

When wiring is difficult, reserve power pads on the board to facilitate flying wires during production.

There should be a separate power socket or pad on the circuit board where the row driver is located.

There should be separate power sockets or pads on the circuit board where the column drivers are located.

When using the non-soldering method (pin header, hole arrangement and cable arrangement) for power supply and row line connection, the current of each pin is not more than 1A, and each connection has at least two pins.

For the user’s existing light board, it will be discussed separately.

It is recommended that the line tube be placed within 1/3 of the entire unit board in the middle of the line.

For the outdoor screen, if the lamp board driver board is separated, the line tube should be placed near the line lead-in pin.

(4) Requirements for ground wire

The ground line width of the digital part is >=50mil.

The ground line of the column drive part should be wider than the power line of the row drive, and it is recommended to be more than 1.5 times the width of the power line.

The ground wire of the unit board should be arranged in a checkerboard shape, and the branches should be connected.

The driver part is covered with copper, and the digital part is covered with grid. The distance between the ground and other parts is set to more than 20mil. The line width of the grid ground is 25mil, and the center spacing is 40mil.

When laying the floor, avoid dead corners without loops. After the paving is completed, the divided parts will be connected by manual paving.

Put the test ground pin on the power inlet for the analog ground.

The digital ground is placed between the input pin header, the output pin header and the 9702 and the test ground pin.

(5) Requirements for capacitors

Put 100u electrolytic capacitors and 104 capacitors on the power inlets of the drive part and the digital part.

Place a 100u electrolytic capacitor at the branch inlet and end of the power cord.

It is recommended to leave a 100u electrolytic capacitor near the line driver chip.

The position of 104 capacitors is left between the power pins of the serial-to-parallel driver chip and the ground.

(6) Chip power pin outlet

For serial-to-parallel chips, the power pin out of the row driver chip is at least as wide as the pin pad.

(7) Column and signal lines:

The width of the light board of the outdoor screen, the width of the column line and the signal line is >=12mil. When the PCB size is large, the recommended signal line width is 15mil.

In other occasions, it is recommended that the width of column lines and signal lines be 12 mils, at least 10 mils.

The line spacing is not less than the minimum line width.

(8) Vias:

The light board of the outdoor screen, the via parameters are 50 mil and 28 mil.

In other occasions, the recommended via parameters are 50 mil and 28 mil. At least 40 mil, 24 mil.

The spacing between vias and lines is not less than the minimum line width.

The outer diameter of the power mains via <</span>the power line width, the inner diameter of the power mains via>=power line width*1/3. Recommended via inner diameter: 28mil, 40mil.

Large power and ground traces can increase the number of vias.

To ensure soldering, the vias should not be placed on the pads. At least 5mil from the pad.

(9) Welding device pads:

The via holes of the soldering device pads should ensure that there is no problem with the device insertion.

The inner diameter of the common pinhole is 40mil, and the pad hole of the power socket is 60mil.

(10) Mounting holes:

For the unit board using LED modules, the mounting hole should not be located at the junction of the two modules, and there should be no copper foil around the hole to prevent the mounting hole from being connected to the DC ground of the unit board (for the last resort required by the customer, it must be signed by the customer. ).

General components should be placed 3.5mm away from the center of the fixing hole, and relatively high components (such as capacitors, plug-in chips) should be placed more than 5mm away from the center of the fixing hole.

When the user does not have a clear requirement, the cascade pin header and the power socket should be placed 2cm away from the horizontal and vertical connection lines of the fixing hole.

When designing a PCB for a special customer, it is necessary to clarify the customer’s fixing hole location and fixing structure to determine the placement of pin headers, power sockets and other components.

(11) Module

The module boundary cannot place plug-in components.

The module recommends “queue placement” or grid placement to avoid errors.

The PCB edge should be at least 20mil smaller than the module.

The module is built in front of the library, and it is positioned on the back when placed, so that the front pads of other devices can be prevented from being covered by the silk screen of the module boundary.

The center distance of module placement should be point spacing*8. When the module accuracy is too low to guarantee this data, the center distance of the module placement should be confirmed with the customer.

(12) Optimization:

After the layout design is completed, it should be reviewed and optimized.

The width of the power line should be increased, and the ground wire should be arranged in a checkerboard shape as much as possible.

(13) Layout sequence: Before layout, pre-wiring should be performed to adjust the routing of column lines. You can return to modify the schematic diagram and network table to make the routing of column lines the most convenient. When laying out the board, route lines, power and ground lines, cascaded signal lines, and then other lines should be routed first.

(14) After the PCB design is completed, there should be a description of the PCB processing requirements for the unit board, including: PCB thickness requirements, PCB copper foil thickness requirements, PCB minimum line width, PCB minimum spacing, and PCB minimum via parameters. It is convenient to choose the board casting manufacturer during the board casting process.

(15) After the PCB design is completed, a list of components should be made, and various component packages should be clearly marked. If there are components that have reserved positions and do not need to be welded during production, they should be specially indicated. The component list should also include a brief description of soldering precautions.

(16) Silk screen layer

After the design of the cell board is completed, the cell board information is marked on the TOP layer of the cell board, including the board number, basic parameters of the cell board, and completion date.

The unit board should have obvious cascading direction signs at the conspicuous positions of the cascading inlet and the cascading outlet; there should be obvious signs indicating the 1-pin position of the cascading pin header and other pin headers; for the positive and negative poles of the power socket There should be an easy-to-observe +- sign next to the pin, and there should be a clear indication of the soldering direction; for the empty pads designed for jumpers, there should be an obvious net name mark; for the unit board where the light board and the driver board are separated , There should be obvious plug-in direction indications on both the light board and the driver board, or asymmetrical treatment should be done in the design.

For components that are divided into positive and negative poles, the direction of the positive and negative poles should be reflected on the layout. Such as diodes, voltage regulators, electrolytic capacitors, power sockets, etc., and the direction of placement indicates that they cannot be covered after welding;

For the unit board of virtual pixels, in addition to the welding direction of the LED, there should also be an obvious R/G/B mark. For the unit board of the surface-mounted LED lamp that cannot be screen-printed at the bottom, the LED lamp should be explained in detail in the production instructions. arrangement.

In order not to affect the soldering, the characters of the silk screen layer cannot overlap with the pads.

After the drawing is completed, place the name of the IC under the IC; for 62706 or 595, place the logo of its control color next to the IC;

After the PCB design is completed, place optical positioning points on the diagonal of the PCB.

(17) Detection

After the design is completed, DRC testing is required. When converting to PROTEL2.8 after drawing with PROTEL99 and POWERPCB, DRC detection is also required.

When importing into Protel2.8 format after drawing with PowerPCB software, it should be noted that sometimes, the vias on the board will change in size. After using the Protel99 software to draw a picture, import it into the Protel2.8 format, and the vertically placed FILL may be turned into a horizontal placement. These are the things to pay attention to in drawing.

When drawing the PCB, the positive and negative components must be able to reflect the direction of the positive and negative electrodes on the layout. Such as diodes, Zener tubes, electrolytic capacitors, power sockets, etc.

For two-pin components, you must no longer use the common two-pin component library of SIP2 or IDC2, and must use a dedicated component library.

For the power socket or power pad, be sure to mark the network name (or positive and negative signs) on the silk screen layer.

For single-row needles and double-row needles, there should be a clear mark at the position of one foot.

For other components, there must be an obvious 1-pin mark or a welding direction mark.

For unconventional usage, it must be explained in the production instructions.

For the unit board of virtual pixels, in addition to the LED ground welding direction, there must be an obvious R/G/B mark. For the surface-mounted unit board that cannot be screen-printed at the bottom, it should be explained in detail in the production instructions.