Design For Manufacture
Note: all information below is based on our own experience and we don't pretend it to be ultimate of
comprehensive. Your comments and suggestions are welcome.
Cost forming factors in PCB production
- The quantity and size of the PCB
- The Number of Layers - try to route your board with minimum number of layers. Some times
is more cost effective to place some jumpers on the board and to make it single side. Roughly
speaking the cost of double layer = 2 * cost single layer, cost of 4 layers = 2 * cost double
layers. The number of layers always come in pairs i.e. 1-2-4-6-8-10-12, there are some odd layer
stacks as 3 layer board but the price will be same as 4 layer board so what do you gain if you
make your board with 3 layers?
- Effective panelization - the board laminates come in different sizes, most used size
is 1020 mm x 1220 mm (40"x48"). They have to be cut on panels. Each panel must have
technological space around the board area for registration pins, plating holding frames etc.
Each of these operations generate laminate scrap. Some board sizes utilize up to 80% useability
some down to 50%. This would affect your price.
- Manufacturing yeld - here you can save a lot into the design stage. Don't push the
manufacturer's limits. For instance if your manufacturer can produce 4 mils don't route all
your boards with 4 mils if you have space to route them with 40 mils.
- Number of holes - the boards are drilled on sophisticated NC drilling machines.
These machines are quite expensive and the machine time is expensive too, so less holes means
less machine time for drilling and lower cost.
- Number of hole sizes - the slowest operation in drilling is the tool exchange. Usually
the boards are drilled at very high RPM values up to 60-80.000 rpm/min. To change the tool the
machine have to stop the spindle, to wait until the tool stop rotating. To move to the drilling
rack, to place the old tool, to get new tool, to move back to board drill position, to drive the
spindle again and to wait the RPM value to reach the drill RPM setpoint for the new tool. Each
tool change takes approximately the time for drilling 100-200 holes. Try to minimize the number
of drill tools as much as possible. Combine the tools with difference only few mils if your
holes will pass your required tolerances.
- Laminate material - when you intend to manufacture your board in volume the right choice
for the board laminate can save a lot of money. For instance dispite the superior characteristics
of FR-4, all consimer electronics today still is manufactured on old paper FR-2 laminates as they
cost two times less expensive than FR-4.
- Trace width / space requirements - this is in close relation with the manufacturing yield.
For instance if your traces are wide enough (>20mils) the board can be manufactured with etch
resist single silkscreen priniting operation instead of dry film lamination, exposure,
- Special board requirements, controlled impedances etc. - this affects again the
Common design tips
- Check the schematic for errors, duplicated component names etc.
- Check the schematic BOM for matching components in the standard library.
- Create the components which are not in the library:
- Silkscreen Outlines
Don't place silkscreen outlines on the solder pad area
Use silkscreen line widths which meet your PCB manufacturer's requirements
If the board is double sided the plating will decrease the holes with 0,1 mm
The component lead - hole clearance have to be 0,2 - 0,4 mm
If your board will be assembled by automat use clearance in the upper limit.
Clearance > 0,5 mm may cause unfilled pads (especially for single side PCB)
Clearance < 0,3 mm for PTH boards make difficults flux gases to escape and may cause
unfilled pads by machine soldering. (well this pretty well depend on the flux used)
Try to standartize the hole sizes you are using, don't use many drill sizes with 0,1 mm
difference, or be ready to pay for this ;)
If you are designing single side board use bigger pads as they have to keep the component's load.
We recommend you anual rings about 40-50 mils if the board is single side and exposed to vibrations.
Use oblonged or rectangular pads to enlarge the pad area for IC and components with the board is densite.
Use thermal bridges when the pads are in copper area.
The minimum annual ring (pad-hole) have to be = hole + 2 * min track width of your PCB manufacturer.
- Place PCB dimensionins, mount holes, mark on doc layers areas with component height restrictions,
overlaying, assembly etc. Allow sufficient area around the mounting holes.
- Place the components with fixed locations: connectors, switches, buttons, displays etc.
- Use standard gird 50 mils 25 mils 5 mils
- Group the components with many connections between to be close to each other
- The fast signals to be with shortest traces
- Use TOP view when design boards with only PTH components and BOTTOM view when design with only
- Place the ICs on even gird to route the power supply easier
- Place the filtering caps to be closest to the power supply pins
- Don't overlay components
- Place the components at angles different than 0 and 90 degrees only if unavoidable
- Factors which determine the proper track width:
- The current, the operating temperature, the laminate copper thickness - all those
factors have to prevent heating of the board over 130 C.
- The board density: the good designer have to attempt to route the board with as thick
tracks as possible - this easy the PCB manufacture and lower the PCB production cost.
- Track to track, track to pad, pad to pad spaces:
- use wider spaces if high impedance circuit
- use wider spaces if high frequency circuit
- use wider spaces if no clean fluxes or pastes are used
- use wider spaces if the board will work at bad climatic conditions
- use conformal coating if the board will be exposed to humidity, moisture, dust etc
(for instance in automotive)
- Place the components at least 100 mils to board edges (wave machine fingers have not to touch
- The tracks/copper area have to be at least 60 mils from the board edge to prevent short to the
- Even if you are using Autorouter, first route the power supply (the thicker traces)
- Start routing the shiortest tracks then the longer
- Good routing strategy is to route to one side horisontal to the other vertical
- The critical signals have to be routed manual
- Route the analog and digital ground separately
- Don't place vias under the components - they keep flux even after cleaning and may cause
- Place border on all layers, please text which to be readable with the layer orientation to
prevent mirrored board production (especially for single side PCB and PCB with SMT components)
- Try to avoid vias
- Avoid acid traps (tracks at angles less than 90 degrees)
Design rule check & post processing
- First do DRC check to your tightest manufacturer's requirements. If the check pass increase
the min.space rules with say 20% and do DRC again to see where are the "weakness" of your
board. If the new DRC check found only few violations change them, so your board will be
easier for mass production (and less expensive).
- Don't forget to switch ON all necessary layers.
- Check your Gerber files with Gerber viewer (you can find freewares in our Design tool section).