7Study Case

In this section all complete PCB Design Process will be shown by following a real PCB case. The design has been done using Altium Designer Software. Main steps include the following:

- Library Creation: all the symbols for schematic design have to be done and all necessary footprints for PCB design have also to be created before to start the PCB Layout.
- Get all necessary information
  - Mechanical housing information 3D Step format, DXF (scale 1:1), PDF ....... containing inhibit areas for components in TOP and BOTTOM side of the board.
  - Final schematic: containing all connections between components, some rules related to the different nets and explanations about how to proceed with special components.
  - Key components layout recommendations from component manufacturer (this applies to microcontrollers, power components, DDR, and any component requiring special layout)
- Layer stack-up definition: define depending on PCB necessity, density, budget and time to design.

Fig. 6. PCB Layer stack-up definition.

- Import mechanical DXF to Altium special layer (mechanical layer).

Fig. 7. Mechanical layer.

- Define the board shape from DXF in mechanical layer 2 (we will use mechanical 1 for production panel and mechanical 2 for single board design)
- Place the PCB Origin. This is very important and necessary in order to have a good reference point for design, placing the single PCB in the production panel, 3D housing placement and production information generation (gerber, drill) and mounting documentation (pick and place, ODB++ files).

Fig. 8. PCB Origin.

- Draw the inhibit areas for component placement, copper and different height restrictions in TOP and BOTTOM sides (choose any Altium mechanical layers).

Fig. 9. TOP and BOTTOM sides.

- Set all the Design Rules in Altium Designer. It’s possible to set up different rules in order to help with our design. The rules are relative to Electrical and Routing restrictions (clearances), topology, layers to be used, placement, manufacturing, signal integrity and many others. We will choose the corresponding and necessary to success with our design.

Fig. 10. PCB Rules and constrains editor.

- Perform the PCB update from schematic. All the PCB footprints corresponding with schematic symbols will appear in the PCB.

Fig. 11. PCB footprints with schematic symbols.

- Do the component placement. In that design, the target is to get minimum pattern length with only using two layers in order to minimize final product cost. Also the best power dissipation is necessary, so we need to prepare the maximum free space for making thick copper connections.

Fig. 12. 3D Top Side, TOP and BOTTOM sides.

- Place the components with fixed position (from mechanical Design) as LED and Connector.
- Take care with the defined component placement allowed areas.
- Place all components inside each circuit block as near as possible between them.
- Keep enough space for the transistor to control current through led in order to allow the maximum dissipation (high power).
- Place Voltage Dividers close together.
- Check the final placement with the real mechanical housing by embedding 3D step.

Fig. 13. 3D (Top Side), TOP and BOTTOM sides.

- Perform the PCB Routing
  - Sometimes, once start the routing some possible placement improvements are detected, so it means additional 3D checks have to be done for assure no problems with complete product.
  - Many vias are added for improving the thermal dissipation (this is special board where power dissipation is quite important).

Fig. 14. PCB routing.

- Production Panel Design. Must be done to make a quicker and cheaper assembly process. The panel contains many single PCBs with some holes and marks. Dimensions of Panel are defined according to production plant requirements and bare board manufacturer best working panel profitability. The Working panel contains many production panels.

Fig. 15. Production panel design.

- DRC (Design Rule Check) & DFM (Design For Manufacturing) check.
- DRC allows to PCB Designer to detect any possible error and assure the final PCB quality. The checks are done automatically following the stetted up Design rules. Some of the DRC checks are related to following rules:
  - Electrical: Un-Routed Net, Un-Connected Pin, Short-Circuit, Clearances, ....
  - Routing: Copper Width, Via Style, routing layers, differential pairs, ....
  - SMT: distance from any SMD to Copper Plane, Corner, ....
  - Manufacturing: Silk to Solder Mask, Silk to Silk, hole to hole, hole size, ....
  - High Speed: Vias under SMD, Parallel segment, via count, matched lenghts, .....
  - Placement: Maximum height, component clearance, allowed layers, ...
  - Other specific user design rules
- DFM is done by Panel assembly production plant, and reports to PCB Designer any issue affecting the assembly process quality.
- PCB production panel documentation generation for Bare Board manufacturing and assembly:
- Necessary for PCB Bare Board manufacturing
  - Gerber Data
  - Drill Data
  - PCB Specification Sheet
- Necessary for PCB Assembly
  - Gerber & Drill Data
  - Files for SMD solder paste stencil fabrication
  - PCB Specification Sheet
  - PCB assembly information (pdf ‘s for any pcb layer)
  - ODB++ (universal format)
  - Test Points report: for In Circuit Test (ICT) and Functional Test
  - Pick & Place file: for components auto insertion machines