Layout Tipps & Tricks
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.
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.
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
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.
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.
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 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.
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.
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:
How about a webinar on circuit board design?