Layout Tips & Tricks - from developers for developers
In this section, you will find assistance and suggestions on how to design your printed circuit board to meet production requirements and avoid later increased handling and production costs during assembly production.
How about a webinar on circuit board design?
Layout Tipps & Tricks
The placement print helps with measuring and troubleshooting on electronic assemblies. The correct alignment of components can also be easily checked by marking them using placement printing (pin 1). However, due to the ever increasing miniaturization, it should be considered whether such placement printing is still useful. All free copper areas (pads, vias) are left blank by the PCB manufacturer. Thus, poorly positioned prints quickly become illegible.
The extent of the placement print should be minimal, precisely defined and one should consider whether it is really necessary. It should be noted that the paste stencil cannot lie flat on the PCB during placement printing and there is a risk that no clean solder deposit can be printed. Under components, placement printing should be dispensed with entirely.
Test and testability of assemblies
Measures for the final tests and commissioning of the electronic printed circuit boards after the production process should be considered in the design from the beginning.
- Provide trap holes for the PCB (asymmetrical, typ. 3.2 mm, not plated through and not tinned.) Consider keep-out zones!
- Test points in each electrical node; vias can be used as test points provided they have> 0.8mm pad diameter and are not covered.
- Distance of the test points to each other and to the PCB edge > =2.54 mm; In exceptional cases and after consultation, the distance can be reduced to up to 1.27 mm. This leads to higher costs in the test equipment.
- Test points should be placed evenly on the PCB in order to distribute the forces by contact needles in a balanced way.
- For supply voltage networks, several test points should be placed. These should be distributed on the PCB or positioned at the beginning and end of the trace.
- Test points should preferably be placed only on the component-free side or the side with the lowest components.
- In the case of metrologically critical components (low-resistance shunts), a four-wire measurement should be provided.
- Components which have an enable input should be switched to "high" or "low" in the design via a pullup/pulldown. This gives the possibility to deactivate them during the test.
- SMD and THR solder joints must not be used as test points, as they may be contaminated by flux residues. Contacting is then not possible.
- A test point diameter of 1mm, but min. 0.8 mm is recommended.
Solder / Solder
The solder (or brazing tin) is used to join metals by soldering. The solder consists of an alloy of different metals. The melting point of the solder is lower than that of the workpieces to be joined. In the past, lead was contained in many solders. Since 2007, these solders may only be used in exceptional cases in the EU in accordance with the RoHS Directive.
The solder for reflow soldering is applied in paste form. The paste consists of small tin balls and flux. The solder paste is available in different grain sizes. If electronic assemblies are subjected to different soldering processes (reflow, wave and manual soldering), the solder used should be matched so that no undesirable metallurgical effects occur.
General selection criteria for electronic components
Electronic components are selected primarily on the basis of functional requirements. In order to keep total cost of ownership (TCO) low over the complete life cycle of an assembly, the following criteria should be considered in the selection process:
- Long-term unit cost
What is the unit price of the component and what scale prices can be achieved over a longer period?
It is worth consulting suitable databases in advance to check the long-term availability of a component.
- Second Source
Are components available from several sources or can components with several sources be preferred? This ensures long-term availability from different sources.
- Common housing variants
Is a component really only available in a certain package variant from one source? Can another housing variant be used that can be obtained from multiple sources?
- Preferred components
Are there preferred components in the company or at your EMS service provider that can be used? Can a price and availability advantage be achieved from this?
- Component variants
Can the number of component variants be reduced? For example, can capacitors with identical capacitance also have a uniform dielectric strength?
NOTE: Ginzinger electronic systems offers services for the life-cycle check of your assembly to ensure a long-term, economical production of the product.
The production costs of an electronic assembly are determined during development. Many important decisions are made here.
- Is one-sided assembly possible?
Especially if only a few components are to be assembled on the second side of the PCB, production costs can be saved by shifting to only one side.
- Are many different components of the circuit used or can some components and values be standardized?
Reducing the number and variance of components saves setup costs in production.
- Can the packaging of the components, such as rolls, bars or trays, which is optimally suited for later processing already be influenced in the development phase during component selection?
Automatable packages with a higher number of components save storage and production costs.
- Is it possible to use a cheaper chip technology?
LVC standard logic is cheaper than HC, for example.
- Can connectors or relays in THR technology be used?
These can be soldered more cost-effectively and fully automatically in the reflow process. An additionally required THT process is saved.
- Is a higher product class and thus more expensive processes and materials really necessary?
Standards and guidelines are often over-interpreted or additional safety features are built in. These no longer significantly reduce the risk of a system, but greatly increase the costs.
- Are multifunctional problem solutions possible?
- Can a housing also be used as a heat sink, for example?
- Can costly special tools for processing and production be avoided?
Possibly, after minor adjustments, the production step can also be carried out with inexpensive standard tools.
- Are all components also available in the long term?
A timely life cycle check with a suitable database prevents expensive revisions in advance.
- Which components are subject to a particular risk?
Large ceramic capacitors, for example, are sensitive and can break easily in the production process.
- Have all possible component shapes been considered?
Smaller shapes of a component can often be better automated and processed at lower cost.
However, component shapes and pin spacing that are too small can also lead to increased costs. Coordinate in good time with your EMS service provider which build shape will give you the cost optimum from material price and production costs.
panel design & depaneling
A panel is a composite of several printed circuit boards. The PCBs are usually not assembled individually, but in a panel. After assembly, the PCBs are separated, i.e. separated by a depanelizer. In order to optimize the production process, Ginzinger electronic systems will gladly take over the depaneling of your PCB. For this purpose, information about blocked connection areas, keyword "cut outs" and milled edges, may be necessary. The user design will be optimized according to manufacturing aspects.
In the course of the depaneling process, Ginzinger electronic systems also creates the paste stencil for SMT assemblies.
Most assemblies, especially those with complex outer contours, are processed at Ginzinger electronic systems in milled blanks. Compared to scribed blanks, blanks with milled lands are mechanically more stable.Deflection during soldering due to heavy components or variations in scribe depth and the associated defects are thus reduced.
bonding of smt components
There are three restrictions for wave soldering of previously glued SMT components:
Components with a length ≤ 1.2 mm (e.g. component size 0402) cannot be soldered to the shaft. They can no longer be bonded with sufficient safety. Component size 0603 should be avoided in the wave soldering technique, since the process reliability is lower than with larger sizes.
Components with a height > 2.5 mm can easily be washed away by the pressure of the wave or, if they are even taller, they will stick to fixed parts of the wave soldering system. In the case of film capacitors, their heat sensitivity must be taken into account.
Ceramic capacitors above size 0805 should not be wave soldered because of thermal stress.
Common practice is to bond SMT components in a separate process step and solder them together with the THT components on the solder side above the solder wave. Care must be taken to ensure that the SMT components are aligned in the direction of the wave, otherwise solder shadows will lead to unsoldered components. (see figure)
In addition, attention must be paid to possible short-circuits with transverse ICs. ICs with 0.8 mm pitch can still be soldered without solder bridges if the layout is correct for the shaft (existing solder traps and correctly positioned components). Solder traps must be twice as long as the pad and rounded or pointed at the end. (see SO14 in the figure)
If no or rectangular solder traps are used, spilling back solder can lead to solder beads or short circuits between the pins.
With the 0.8 mm pitch, there is a free space of about 0.4 mm between adjacent pads. The practical achievability of the wave soldering minimum depends, among other things, on the local topology of the assembly and the associated flow conditions on the assembly. Tests should be carried out before series production is started. The practical soldering limit for a wave soldering result free of solder bridges with standard equipment is a uniform minimum distance of about 0.4 mm to 0.5 mm.
Gerber data is mandatory for the calculation of a quotation. The printed circuit board manufacturer needs these for quoting. To ensure smooth production, intelligent CAD data should also be provided. All common file formats such as ODB++ , ASCII files or IPC-2581 are supported. The following information defines the requirements for electronics production at Ginzinger electronic systems and is needed for a quick and uncomplicated processing:
Board designation & assembly type (e.g. SMT single/double sided; THT)
PCB dimension (l x w [mm])
Copper layers and thickness Number/assembly
Base material and thickness FR4/xy mm
Color solder resist Standard is green
Assembly print Yes/No/Color
Surface Electroless Nickel-Gold; HAL
Contours fritted Yes/No
Impedance controlled LP Yes/No
IPC-A-610 Class 2 or 3
Component manufacturer fixed bill of materials
Functional test, AOI, climatic test
Test report Yes/No
UL marking of LP Yes/No
Customer specific label Yes/No
The manufacturing data and plans are ideally sent as a ZIP-compressed file to the customer consultancy.
What belongs in the Gerber package?
Copper layers (incl. layer structure description)
Assembly plan for SMT, assembly plan for THT
paste data, drill data
Laser marking TOP/BOT
Optional: placement print, BlueMask, test point plan
Part reference TOP/BOT, X coordinates [mm], Y coordinates [mm], Rotation [°]
Test point data
Net name or catch holes TOP/BOT, X coordinates [mm], Y coordinates [mm], test point size [mm]
Component reference number(s) - corresponding to assembly plan
Description incl. tolerance or manufacturer and manufacturer designation
Type of construction
Number of pieces per assembly
NOTE: Preference is given to parts lists in XLS and CSV formats.
Circuit diagram as PDF, test instruction and if available the impedance calculation of the PCB.
Material to be provided
NOTE: Providing materials should ideally be avoided, as suboptimal component packaging can result in significant additional costs.
Printed circuit boards - materials & surfaces
The desired PCB material, solder resist, and surface finish is defined by the customer. Most commonly used surfaces are electroless tin, HAL(lead free) or electroless nickel/gold. We will give you an overview of the most common materials and their advantages and disadvantages:
Deposition of an electroless tin layer up to a maximum of 1.2 µm. The minimum is 0.6 µm.
--> Immersion tin is recommended by Ginzinger electronic systems.
very good soldering properties
good corrosion protection for underlying copper
good press-in properties
no metallurgical bond to the copper layer
narrowed process window for brazing processes
use of thiourea (environmentally harmful)
limited shelf life due to thin layer thickness (< 6 months)
only 2-3 reflow cycles
HAL (Lead Free)
HAL (Hot Air Levelling) is the most proven method for applying tin as a PCB surface. Layer thicknesses are from 1-20 µm, occasionally up to 50 µm.
good soldering properties
Good shelf life (at least 12 months)
limited suitability for fine pitch
copper is deposited
thermal stress for the printed circuit board
Note: Pitch is the average distance between the connecting legs of electronic components. If this distance is less than 0.5mm, it is referred to as fine pitch.
Electroless nickel/gold is also known as ENIG = Electroless Nickel Immersion Gold. In addition to full-surface nickel/gold plating, partial nickel/gold plating is also possible when a suitable solder resist system is used.
very good shelf life (>12 months)
very good for fine pitch
good press-in properties
resistant to environmental influences
limitations with various base materials (e.g. PTFE)
high process temperatures (electroless nickel approx. 90°C for approx. 20 minutes)
brittleness of the intermetallic phase with small solder deposit
Acceptance criteria according to IPC-A-610 and layout
During layout, minimum distances between pads and traces are typically determined based on dielectric strength. Often the IPC A-610 acceptance criteria are not taken into account. An example: a chip component of size 0805 is 2.0 x 1.25 mm long or wide. according to class 2, an overhang of the component of 0.62 mm and for class 3 of 0.31 mm would be IPC-compliant, provided that the minimum electrical isolation distance is not offset.
The minimum electrical insulation distance is usually not known during production. For this reason, half the distance (relative to the outer edge of the pad) to the next potential (conductor track, pad) is usually assumed here.
PCB size and strength
Common PCB thicknesses at Ginzinger electronic systems are between 1 and 2 mm. Deviations from the common PCB thicknesses have to be clarified individually.
The IPC class of an electronic assembly is determined by the area of application of the end product. The following classes are defined in IPC-A-610:
Class 1 - General Electronic Products.
This includes products for which the main requirement is the functioning of the fully assembled assembly.
Class 2 - Electronic products with higher requirements (Dedicated Service Electronic Products)
This includes products where continuous function and extended life are required and uninterrupted operation is desired but not critical. Typically, the operating environment does not cause failures during operation.
Class 3 - High Performance Electronic Products.
This includes all products where continuous, high performance or on-demand power delivery is essential. Functional failure cannot be tolerated. The operating environment of the equipment may be unusually harsh. The equipment must function when needed, such as for life support or other critical systems.
NOTE: Class 1 production is not performed at Ginzinger electronic systems.
Soldering & Soldering Processes
To make a mechanically and electrically reliable brazed joint, time and temperature are required. Soldering does not produce a metallurgical bond as in welding, but instead creates a joint in which different alloys or metals diffuse into each other. This creates an intermetallic phase (IMP). The goal is to achieve the ideal thickness of this IMP. If it is too narrow, a cold solder joint results; if it is too thick, it becomes brittle.
Here, the layout lays the foundation for the subsequent achievement of an optimal solder joint, especially with regard to heat requirement, connection surfaces and heat input or heat dissipation. There are various methods for soldering, but a nitrogen tunnel is used in all machine soldering processes to achieve the best possible soldering result.
This process is used to solder SMT and THR components on the top or bottom side. The solder paste is deposited at the solder joint by means of stencil printing. All components are automatically loaded by the placement machine and the loaded assembly is transported via a transport system to a reflow (or vapor phase) soldering system.
If components are assembled on both sides, care must be taken to ensure that heavy and temperature-sensitive components are always placed on one side (electrolytic capacitors, light-emitting diodes, SMC diodes, connectors, etc.). Otherwise, these components must be glued in an additional process step.
In wave soldering, the assembled component to be soldered is transported over a solder wave (=turbulent bath) of liquid tin. Beforehand, flux is applied from below, which is activated in the preheating phase. This breaks down existing oxide layers and heats the assembly to the required base temperature. This is followed by soldering and cooling of the assembly.
Wave soldering is used to solder THT components on the TOP side and SMT components on the BOT side. SMT components on the BOT side must first be bonded to the PCB in an upstream process step.
Design parameters during soldering
Design parameters for soldering SMT components
The IPC-A-610 acceptance criteria for electronic assemblies describe how solder joints should look. Maximum side overhang, end overhang, minimum and maximum length, width and height of the solder joint, solder gap thickness, etc. are listed here. However, the values vary from package to package. The developer can mainly influence the solder joint in terms of component connection type, pad size, pad spacing and PCB surface.
As a developer, you should always be critical of pad suggestions in the component data sheet. Tip: Draw connections in the footprint and carry out a "proportional consideration": Can the pins on the surface be soldered at all? Is there too much protrusion from the pad? Are the pads too small?
Calculation tools can also help here, such as "Proportional SMD Reference Calculator" from the Fachverband für Design, Leiterplatten- und Elektronikfertigung (FED), "PCB Footprint Expert" or "Footprint Designer" from the ECAD systems.
The connection of vias to pads should generally be made via traces. This avoids solder migration and the resulting formation of an insufficient solder meniscus.
The distance between via and pad must be large enough to be able to separate them by a bar of solder resist. The smallest solder resist web that can be realized varies depending on the PCB manufacturer.
Caution: If vias with a different potential are located under a component, there is a risk of the minimum electrical distance being undercut (short circuit).
NOTE: Through-holes under components can be problematic during the wave soldering process.
Connection of SMT components
The connection of pads to tracks should never be made over the entire surface or over wide tracks, unless this is electrically or thermally absolutely necessary.
On the one hand, this can lead to a "lean" solder joint and, on the other hand, to defective solder joints (tombstoning) due to increased heat dissipation (heat sink). This can be especially critical with BGAs, since their solder joints can only be inspected and detected by X-ray analysis.
NOTE: The smaller the component, the more critical these negative effects are.
Heat Traps & Heat Sinks
Large copper areas in PCBs dissipate heat and can lead to insufficient/uneven melting of the solder paste, or insufficient through-hole. In this case, the through-hole is not completely filled by the solder. Similarly, large components can dissipate an above-average amount of heat, leading to an unsatisfactory soldering result.
In the case of THT and SMT components with an increased heat requirement at one or more connections, the heat input can be increased by means of an appropriate design of the PCB. The same applies to the placement of vias in the immediate vicinity of components. In both cases, it is important to consider from which side the heat input is coming. Unused pads should be removed on inner layers ("non functional pad removal"). In multilayers, layers with large copper areas should be placed as close as possible to the surface - on which the heat input occurs.
NOTE: The greater the distance between pad and surrounding copper, the better the heat trap.
An additional possibility is the use of different pad areas on the TOP or BOT side for wave soldering. With large pads, there is good heat input or heat dissipation. An opposite effect occurs with smaller pads. Solder penetration can be improved by using the appropriate combination (large pad on the solder source side, small pad on the solder target side).
Tips and tricks from 30 years of experience in electronics production can be found in our EMS Design Guide. Our practical little helper is now available in a new and completely revised 4th edition. For free pre-order: