PowerPCB circuit board design specifications

fighting

PowerPCB circuit board design specifications [Copy link]

Data compilation: dunleavy [ Print ] [ Return ]

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

2 Design Process
The design process of PCB 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 input the netlist. One is to use the OLE PowerPCB Connection function of PowerLogic, select Send Netlist, and apply the OLE function to keep the schematic and PCB 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.

2.2 Rule Setting
If the PCB design rules have been set in the schematic design stage, there is no need to set these rules again, because when the netlist is input, the design rules have been input into PowerPCB along with the netlist. If the design rules are modified, the schematic must be synchronized to ensure the consistency between the schematic and the PCB. In addition to the design rules and layer definitions, there are some rules that need to be set, such as Pad Stacks, which requires modifying the size of standard vias. 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 the default startup file named Default.stp. After the netlist is input, the power network and ground are assigned to the power layer and ground layer according to the actual design situation, and other advanced rules are set. 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 the consistency of the rules between the schematic and the PCB.
2.3 Component Layout
After the netlist is input, all components will be placed at the zero point of the workspace and overlapped. 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. Use the tool to draw the board outline according to the structural dimensions of the printed circuit board.
2. Disperse components, and the components will be arranged around the board edge.
3. Move and rotate the components one by one, place them within the board edge, and arrange them neatly according to certain rules.
2.3.2 Automatic layout
PowerPCB provides automatic layout and automatic local cluster layout, but for most designs, the effect is not ideal and is not recommended.
2.3.3 Notes
a. The first principle of layout is to ensure the routing pass rate. When moving devices, pay attention to the connection of flying wires and put devices with connection relationships together
b. Digital devices and analog devices should be separated and kept as far away as possible
c. Decoupling capacitors should be as close to the VCC of the device as possible
d. When placing devices, consider future welding and do not place them too densely
e. Use the Array and Union functions provided by the software more often to improve the efficiency of layout
2.4 Wiring
There are also two ways of wiring, manual wiring and automatic wiring. The manual routing function provided by PowerPCB is very powerful, including automatic pushing and online design rule checking (DRC). Automatic routing is performed by Specctra's routing engine. Usually these two methods are used in combination, and the common steps are manual-automatic-manual.

2.4.1 Manual routing
1. Before automatic routing, manually route some important networks, such as high-frequency clocks, main power supplies, etc. These networks often have special requirements for routing distance, line width, line spacing, shielding, etc.; some other special packages, such as BGA, are difficult to route regularly by automatic routing, and manual routing is also required.
2. After automatic routing, manual routing is also required to adjust the routing of the PCB.
2.4.2 Automatic routing
After manual routing is completed, the remaining networks are handed over to the automatic router for routing. Select Tools->SPECCTRA, start the interface of the Specctra router, set up the DO file, and press Continue to start the automatic routing of the Specctra router. After the end, if the routing rate is 100%, then you can manually adjust the routing; if it is less than 100%, it means that there is a problem with the layout or manual routing, and you need to adjust the layout or manual routing until all are routed.

2.4.3 Notes
a. Make the power and ground wires as thick as possible
b. Connect the decoupling capacitors directly to VCC as much as possible
c. When setting the DO file of Specctra, first add the command Protect all wires to protect the manually routed wires from being rerouted by the automatic router
d. If there is a mixed power layer, the layer should be defined as Split/mixed Plane and split before routing. After routing, use Plane Connect of Pour Manager to cover copper
e. Set all device pins to hot pad mode. The method is to set Filter to Pins, select all pins, modify the properties, and check the Thermal option
f. Turn on the DRC option when manually routing and use dynamic routing (Dynamic Route)
2.5 Check
The items to be checked are Clearance, Connectivity, High Speed and Power Plane. These items can be selected by Tools->Verify Design. If high speed rules are set, they must be checked, otherwise this item can be skipped. If errors are found, the layout and routing must be modified.
Note:
Some errors can be ignored. For example, part of the Outline of some connectors is placed outside the board frame, which will cause errors when checking the spacing. In addition, copper must be re-coated every time the routing and vias are modified.

2.6 Review
The review is based on the "PCB Checklist", which includes design rules, layer definition, line width, spacing, pads, and via settings; it also focuses on reviewing the rationality of device layout, routing of power and ground networks, routing and shielding of high-speed clock networks, placement and connection of decoupling capacitors, etc. If the review fails, the designer must modify the layout and wiring. After passing, the reviewer and designer sign respectively.

2.7 Design Output
PCB design can be output to a printer or output to a photolithography file. The printer can print the PCB in layers, which is convenient for designers and reviewers to check; the photolithography file is handed over to the board manufacturer to produce the printed board. The output of the photolithography file is very important and is related to the success or failure of this design. The following will focus on the precautions for outputting the photolithography file.

a. The layers that need to be output include the wiring layer (including the top layer, bottom layer, and middle wiring layer), the power layer (including the VCC layer and the GND layer), the silk screen layer (including the top silk screen and the bottom silk screen), the solder mask layer (including the top solder mask and the bottom solder mask), and a drilling file (NC Drill) needs to be generated .
b. If the power layer is set to Split/Mixed,
select Routing in the Document item of the Add Document window, and before each output of the photolithography file, use the
Plane Connect of the Pour Manager to copper coat the PCB diagram; if it is set to CAM
Plane, select Plane, and 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 Aperture value 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, and select Outline, Text, and Line of the top (bottom) and silk screen layers.
f. When setting the layer of solder mask, select vias to indicate no solder mask on vias, and do not select vias to indicate home solder mask, 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 photolithography files are output, open and print them with CAM350, and the designer and reviewer will check them according to the "PCB Checklist"