PCB Technical - Power PCB design specification

1. The purpose of this document is to explain the process and some precautions of PCB design using the PCB design software powerpcb of pads, provide design specifications for designers of a working group, and facilitate communication and mutual inspection among designers.

2. Design process

The design process of PCB is divided into six steps: net list input, rule setting, component layout, wiring, inspection, recheck and output

2.1. Net list input

There are two methods for net list input. One is to use the ole powerpcb connection function of PowerLogic, select Send netlist, and apply the ole function to keep the consistency between the schematic diagram and PCB diagram at any time, so as to minimize the possibility of error.

Another method is to directly load the netlist in powerpcb, select File - > import, and input the netlist generated by the schematic diagram.

2.2. Rule setting

If the PCB design rules have been set in the schematic design stage, you don't need to set these rules anymore, because the design rules have been entered into powerpcb with the netlist when inputting the netlist. If the design rules are modified, the schematic must be synchronized to ensure the consistency between the schematic and PCB. In addition to design rules and layer definitions, some rules need to be set, such as pad stacks, and the size of standard vias needs to be modified. If the designer creates a new pad or via, be sure to add layer 25.

Note: PCB design rules, layer definitions, via settings and cam output settings have been made into default startup files with the name of default.stp. After the net list is entered, the power network and ground are allocated to the power layer and stratum according to the actual situation of the design, and other high-level rules are set. After all rules are set, in PowerLogic, use the rules from PCB function of OLE powerpcb connection to update the rule settings in the schematic diagram to ensure that the rules of the schematic diagram and PCB diagram are consistent.

2.3. Component layout

After entering the net list, all components will be placed at the zero point of the work area and overlapped together. The next step is to separate these components and place them neatly according to some rules, that is, component layout. Powerpcb provides two methods, manual layout and automatic layout.

2.3.1 manual layout

(1) Draw the board outline according to the structural dimension of the tool printed board.

(2) . disperse components, and the components will be arranged around the board edge.

(3) Move and rotate the components one by one, put them within the board edge, and place them neatly according to certain rules.

2.3.2 automatic layout

Powerpcb provides automatic layout and automatic local cluster layout, but the effect is not ideal for most designs and is not recommended.

2.3.3 precautions

a. The primary principle of the layout is to ensure the wiring throughput. Pay attention to the connection of flying wires when moving devices, and put the devices with connection relationship together

b. Digital devices and analog devices shall be separated as far as possible from C. the decoupling capacitor shall be as close to the VCC of the device as possible

d. When placing devices, future welding shall be considered and not too dense

e. Use the array and union functions provided by the software to improve the efficiency of layout

2.4 there are also two ways of wiring, manual wiring and automatic wiring.

Powerpcb provides powerful manual wiring functions, including automatic pushing and online design rule checking (DRC). Automatic wiring is carried out by specctra's wiring engine. Usually, the two methods are used together. The common steps are manual automatic manual.

2.4.1. Manual wiring

(1) Before automatic wiring, manually lay some important networks, such as high-frequency clock, main power supply, etc. these networks often have special requirements for routing distance, line width, line spacing, shielding, etc

Requirements for; In addition, for some special packages, such as BGA, automatic wiring is difficult to be arranged regularly, and manual wiring should also be used.

(2) After automatic wiring, the routing of PCB shall be adjusted by manual wiring.

2.4.2. After the automatic wiring and manual wiring are completed, the remaining network will be handed over to the automatic router.

Select tools - > specctra, start the interface of specctra router, set the do file, and press continue to start the automatic routing of specctra router. After that, if the routing rate is 100%, you can manually adjust the routing; If it is less than 100%, it indicates that there is a problem with the layout or manual wiring, and the layout or manual wiring needs to be adjusted until it is fully deployed.

2.4.3 precautions

a. The power line and ground wire shall be thickened as much as possible

b. The decoupling capacitor shall be directly connected with VCC as far as possible

c. When setting specctra's do file, first add the protect all wires command to protect the manually laid wires from being re laid by the automatic wiring device

d. If there is a hybrid power supply layer, it should be defined as split / mixed plane. Divide it before wiring. After wiring, use the plane connect of pour manager for copper cladding

e. Set all device pins to hot pad mode by setting filter to pins, selecting all pins, modifying attributes, and checking before thermal option

f. When routing manually, turn on the DRC option and use dynamic route

2.5 inspection

The items to be checked include clearance, connectivity, high speed rule and plane. These items can be checked by selecting tools - > verify design. If the high-speed rule is set, it must be checked, otherwise this item can be skipped. If errors are detected, the layout and routing must be modified.

Note: some errors can be ignored. For example, a part of the outline of some connectors is placed outside the board frame, and an error will occur when checking the spacing; In addition, copper shall be coated again every time the wiring and vias are modified.

2.6 recheck

Recheck according to the "PCB Checklist", including design rules, layer definition, line width, spacing, pad and via settings; We should also focus on rechecking the rationality of device layout, the routing of power supply and ground wire network, the routing and shielding of high-speed clock network, the placement and connection of decoupling capacitors, etc. If the recheck is unqualified, the designer shall modify the layout and wiring. After it is qualified, the rechecker and the designer shall sign respectively.

2.7 design output

PCB design can be output to printer or photo file. The printer can print the PCB layer by layer, which is convenient for the designer and reviewer to check; The photo drawing documents shall be handed over to the board manufacturer to produce the printed board. The output of photo file is very important, which is related to the success or failure of this design. The following will focus on the precautions for outputting photo file.

a. The layers to be output include wiring layer (including top layer, bottom layer and intermediate wiring layer), power layer (including VCC layer and GND layer), silk screen layer (including top layer silk screen and bottom layer silk screen), solder resist layer (including top layer solder resist and bottom layer solder resist), and also generate drilling file (NC drill)

b. If the power layer is set to split / mixed, select routing in the document item of the add document window, and copper the PCB diagram using the plane connect of pour manager before outputting the photo file every time; If it is set as cam plane, select plane. When setting the layer item, add layer25, and select pads and vias in layer25

c. In the device setup window (press device setup), change the value of aperture to 199

d. When setting the layer of each layer, select board outline

e. When setting the layer of the silk screen layer, do not select part type, but select the outline, text and line of the top layer (bottom layer) and the silk screen layer

f. When setting the layer of solder resist layer, selecting via means no solder resist is added to the via, and not selecting via means no solder resist, which is determined according to the specific situation

g. When generating drilling files, use the default settings of powerpcb without making any changes

h. After all photo files are output, open and print them with CAM350, and the designer and reviewer shall check them according to the "PCB Checklist"