PCB News - The general process of PCB board LAYOUT

1 Overview

The purpose of this document is to explain the process and some precautions for printed board design using PADS's printed board design software PowerPCB, and to provide design specifications for designers in a working group to facilitate communication and mutual inspection between designers.

2. Design process

The PCB design process is divided into six steps: netlist input, rule setting, component layout, wiring, inspection, review, and output.

2.1 Netlist input

There are two ways to enter the netlist. One is to use PowerLogic's OLE PowerPCB Connection function, select Send Netlist, and use the OLE function to keep the schematic diagram and PCB diagram consistent at any time to minimize the possibility of errors. Another method is to load the netlist directly in PowerPCB, select File->Import, and input the netlist generated by the schematic diagram.

2.2 Rule settings

If the PCB design rules have been set in the schematic design stage, there is no need to set these rules, because when the netlist is input, the design rules have been imported into PowerPCB along with the netlist. If the design rules are modified, the schematic diagram must be synchronized to ensure that the schematic diagram is consistent with the PCB board. In addition to the design rules and layer definitions, there are some rules that need to be set, such as Pad Stacks, which requires modification of the size of standard vias. If the designer creates a new pad or via, layer 25 must be added.

Notice:

PCB design rules, layer definitions, via settings, and CAM output settings have been made into the default startup file, named Default.stp. After the netlist is input, according to the actual situation of the design, assign the power network and ground to the power layer and ground layer, And set up other advanced rules. After all the rules are set, in PowerLogic, use the Rules From PCB function of OLE PowerPCB Connection to update the rule settings in the schematic to ensure that the rules of the schematic and PCB are consistent.

2.3 Component layout

After the netlist is entered, 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 arrange them neatly according to some rules, that is, component layout. PowerPCB provides two methods, manual layout and automatic layout.

2.3.1 Manual layout

a. Draw the board outline for the structural dimensions of the printed board of the tool.

b. Disperse the components (Disperse Components), the components will be arranged around the edge of the board.

c. Move and rotate the components one by one, put them inside the edge of the board, and place them neatly according to certain rules.

2.3.2 Auto Layout

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

2.3.3 Matters needing attention

a. The first principle of the layout is to ensure the wiring rate, pay attention to the connection of the flying leads when moving the device, and put the connected devices together

b. Separate digital devices from analog devices and keep them as far away as possible

c. The decoupling capacitor is as close as possible to the VCC of the device

d. When placing the device, consider future soldering, not too dense

e. Use the Array and Union functions provided by the software more to improve layout efficiency

2.4 Wiring

There are also two ways of wiring, manual wiring and automatic wiring. The manual wiring function provided by PowerPCB is very powerful, including automatic pushing and online design rule checking (DRC). Automatic wiring is performed by Specctra's wiring engine. Usually these two methods are used together. The common steps are manual-automatic-manual.

2.4.1 Manual wiring

a. Before automatic wiring, first hand-lay some important networks, such as high-frequency clocks, main power supplies, etc. These networks often have special requirements for wiring distance, line width, line spacing, shielding, etc.; in addition, some special packaging, Such as BGA, it is difficult to arrange automatic wiring regularly, and manual wiring must be used.

b. After the automatic wiring, the PCB wiring must be adjusted by manual wiring.

2.4.2 Automatic wiring

After the manual wiring is over, the remaining network is handed over to the automatic router for cloth. Select Tools->SPECCTRA, start the interface of the Specctra router, set the DO file, and press Continue to start the automatic wiring of the Specctra router. After the completion, if the wiring rate is 100%, then you can manually adjust the wiring; if not If it reaches 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 all the connections are made.

2.4.3 Matters needing attention

a. Make the power cord and ground wire as thick as possible

b. Try to connect the decoupling capacitor directly to VCC

c. When setting the DO file of Specctra, first add the Protect all wires command to protect the manually clothed wires from being redistributed by the automatic router

d. If there is a mixed power layer, you should define the layer as Split/mixed Plane, divide it before wiring, and after wiring, use Pour Manager's Plane Connect for copper pour

e. Set all device pins to thermal pad mode by setting Filter to Pins, and select all pins,

Modify the properties, tick the Thermal option

f. When manually routing, turn on the DRC option and use dynamic routing (Dynamic Route)

2.5 Inspection

The items to be checked include Clearance, Connectivity, High Speed and Plane. These items can be selected by Tools->Verify Design. If the high-speed rule is set, it must be checked, otherwise you can skip this item. If errors are detected, the layout and wiring must be modified.

Notice:

Some errors can be ignored. For example, a part of the outline of some connectors is placed outside the board frame, and errors will occur when checking the spacing; in addition, each time the traces and vias are modified, the copper must be re-plated.

2.6 Review

The review is based on the "PCB checklist", which includes design rules, layer definitions, line widths, spacing, pads, and via settings; also focus on reviewing the rationality of the device layout, the routing of power and ground networks, and high-speed clock networks. The wiring and shielding, the placement and connection of decoupling capacitors, etc. If the recheck is unqualified, the designer shall modify the layout and wiring. After passing, the rechecker and the designer shall sign separately.

2.7 Design output

The PCB design can be exported to a printer or a gerber file. The printer can print the PCB in layers, which is convenient for designers and reviewers to check; the gerber file is handed over to the board manufacturer to produce the printed board. The output of the gerber file is very important. It is related to the success or failure of this design. The following will focus on the matters needing attention when outputting the gerber file.

a. The layers that need to be output include wiring layers (including top, bottom, and middle wiring layers), power layers (including VCC layers and GND layers), silk screen layers (including top and bottom silk screens), and solder masks (including top solder masks) And bottom layer solder mask), and also generate a drilling file (NC Drill)

b. If the power layer is set to Split/Mixed, then select Routing in the Document item of the Add Document window, and each time the gerber file is output, you must use Pour Manager's Plane Connect to pour copper on the PCB diagram; if it is set to 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 the Board Outline

e. When setting the Layer of the silk screen layer, do not select Part Type, select the top layer (bottom layer) and Outline, Text, Line of the silk screen layer

f. When setting the layer of the solder mask layer, select vias to indicate that no solder mask is added to the vias, and not to select vias to indicate solder masks, depending on the specific situation.

g. When generating drilling files, use the default settings of PowerPCB and do not make any changes

h. After all gerbera files are output, open and print them with CAM350, and check them by the designer and reviewer according to the "PCB checklist"