5. Constraint Definition
[ Click above image for a larger view ]
PCB design constraints can be classified into Mechanical constraints, Electrical constraints, Design for Manufacturability (DFM) constraints and Design for Testability (DFT) constraints. The PCB constraint editor available in Altium designer is shown above.
Mechanical constraints generally involves restrictions such as positions of connectors, LEDs, LCD display, mounting holes etc., component height restrictions, Board shape and size etc.
Electrical constraints are related to the actual circuit that is being layout on the PCB. These constraints can be pre-set in the CAD software so that while designing the layout, the software will indicate whenever there is a violation of the rules set. Limits such as trace width, trace to trace clearance, trace to pad clearance, pad to pad clearance, pad/trace clearance to board edge etc., can be set using the constraints editor. Additionally specific constraints such as impedance control for high speed lines, differential trace routing, bus routing etc., can also be set. Presetting such constraints will reduce the design cycle time by reducing the number of iterations.
Design for Fabrication (DFF) and Design for Assembly (DFA) together make up Design for Manufacturability (DFM). Complying with DFM constraints will mean that the PCB layout design will be manufacturable. The objective of DFM is to minimize assembly failures and also reduce cost. Some of the critical DFM guidelines for PCB design are listed below:
- Components selected verified for obsolescence and guaranteed availability for atleast the next five years
- Distance between surface mount and plated through hole (PTH) components are adequate
- Components are placed with a minimum clearance of 1.5mm (IPC 2221) from the edge of the board
- Orientation symbols for components to be provided, for example pin no.1 indication for connectors and ICS, Anode/Cathode indication for diodes, Positive/negative indication for polar components like electrolytic capacitors
- Connections to internal plane layers are made through thermal pads
- Avoid acid traps and slivers
- Fix minimum trace width and clearance after confirming with the fabrication house
- Proper solder mask definition for component pads
- Layer stack design should be symmetrical to minimize the risk of warpage of the board
- Balance copper area distribution if possible
- Use panelization to minimize wastage of the base material
- Aspect ratio for a PCB is defined as the ratio of the board thickness to the drill size. Ensuring that the aspect ratio is < 10:1, makes sure that the PCB is manufacturable. It would also do well to confirm with the intended Fab house. Smaller ratios result in more uniform plating in hole.
- Use standard copper thickness of 0.5 oz unless otherwise specified.
- Check with Fab house for minimum thickness of legend text
- Use a minimum of 3 board fiducials and if there are components with pad pitch ≤ 10 mils, use component fiducials as well. Board fiducials are placed at the corners and component fiducials are placed near pin no.1 of the component.
- Check for oversized or overlapping solder mask
- As far as possible component placement should be restricted to a single side and orientation of components should be in the same direction.
- Select the optimum PCB surface finish for the corresponding application
Design for Testability constraints intend to make the PCB capable of being tested, both functional testing and In-Circuit Testing (ICT). Ideally, a 100% test point coverage is desirable. But space constraints on the PCB not allowing, it is then the discretion of the designer to decide which electrical nodes require assignment of test points. Functional testing is intended to validate the electrical design functionality and ICT is intended to detect any manufacturing defects. Both functional testers and ICT access the PCB under test through a Bed-of-nails fixture and connectors. The test points provided on the PCB serve as access points for the testers and hence the test points –
- Should be on a grid of not less than 100 mils (1 mil = 0.001”)
- Should be accessible from the bottom side of the PCB
UP NEXT:
Component Placement and Routing
