PP logo


Electronic design and prototype development.

POUL PETERSEN - or PP - is a minor, highly specialized firm, exclusively dedicated to advanced electronic design and development - mainly within the analogue field of pro-audio and studio equipment.

One of my services is PCB lay-out for low frequency electronics, both singlelayer and multilayer PCBs for leaded as well as SMD components.
I can supply the documentation for PCB manufacturing or I can supply the PCBs - optionally with components - for prototypes and in low volumes.

This page describes the information I require in order to create a PCB lay-out from a schematic in the most economical way, and also lists the documentation I supply with a PCB design.


PCB design flow

This section describes the design flow for a double sided PCB, where all relevant information is available prior to the design phase. The section is included to give an understanding of why I request so much information before starting a PCB lay-out.

A PCAD schematic database is made from a number of symbols, connected by wires. The symbols are picked from a symbol library or created as needed.
A PCAD PCB database is made from a number of parts, connected by traces. The parts are picked from a parts library or created as needed.
A cross reference file defines how the symbols from the schematic database relates to the parts in the PCB database.

Design flow:
Creation of symbols and parts that are not in my present component libraries.
Drawing of a schematic with symbols from the symbol library - optionally on top of a scanned schematic drawing.
If symbol and part relations are different from those in my standard library, a copy of my standard cross reference file is modified for use with this PCB.
Mark up of individual symbols, that should use other parts than defined in the cross reference file.
Mark up of connections that require wider traces or clearances than the default rules for the PCB.
Mechanical drawing of the PCB with markings for mechanical components like screws, connectors, potmeters, switches, displays, etc.
If the database with the PCB's mechanical drawing is in metric format, it is translated into a drawing in inch format.
Electrical Rules Check (ERC) of the schematic database to check for floating inputs, unconnected supplies and shorted outputs.
The schematic is transferred into an electrically equivalent PCB database based on the PCB's mechanical drawing.
Mechanical components are manually placed in the PCB database.
Components, that are not on the schematic (screws etc.), are added to the PCB database.
Initial markup of PCB areas for text, logo etc.
The remaining components are placed automatically or manually.
Component placement optimization. This is mainly done by swapping identical gates between sections within the packages or between the packages while searching for minimal connection density over the entire PCB. For PCBs with a large number of identical components, this can be done automatically, but otherwise some manual work is involved. For PCBs where the visual impression is important, this is done manually as the program does not know about component colors and the like.
The PCB's traces are routed automatically or manually depending on requirements.
Visual check for placement of text and check that text is not in an area with many via holes.
The schematic is updated if the pin numbers have changed due to component placement optimization.
If the PCB is to use x-y part numbering, the parts are renumbered and the new reference designators are automatically back annotated to the schematic.
Component reference designator texts are placed on the PCB, starting with key components like test points and connectors.
Final update of all additional text in the schematic and PCB databases.
Design Rules Check (DRC) of the PCB database to check for wire widths and clearances.
Ground planes are added to the PCB database as required. This is done almost automatically.
Design Rules Check (DRC) of the PCB database to check for wire widths and clearances.
The graphics for the board outline drawing is added to the PCB database.
The parts list for the PCB is created.
The documentation for the PCB manufacturing is created. This includes HPGL plot files, Gerber files, Excellon drill file, component placement file and a PCB specification.
The documentation for the PCB manufacturing is checked manually.
All relevant files are copied and stored for back-up in 2 physical locations.

Required information

As much as possible of the following information should (if relevant) be available prior to starting a PCB lay-out:
Schematic diagram
PCAD can import a number of schematic file formats, but the most reliable method is to use a printed schematic or a file in HPGL file format as a template for the PCAD schematic.
The documentation must clearly state:
  • If sections of the circuit require increased clearances due to high voltages. This is obvious in many cases, but for example where a relay contact is connected to 2 spade terminals, it may not be.
  • If wider traces and larger vias are required due to high currents or low impedance requirements.
  • If components require heatsinking.
If there is any doubt if a specific part of the circuit is required, include it initially, as it is always easier to remove a part of the circuit than to add it to an existing lay-out.
If handwritten documentation is supplied, please be very careful about the typing; errors at this stage may flow through the entire design.
Parts list
The parts list should clearly describe the type of components to be used, preferably by stating manufacturer and type number.
I prefer the parts list in plain ASCII format or on paper, but I can read most common file formats.
If more than one type is listed for a specific component, it must be clearly stated, if I can choose between the types or if the PCB must accept both types.
If handwritten documentation is supplied, please be very careful about the typing; errors at this stage may flow through the entire design.
Data sheets for special components
The data sheets should contain:
  • An exact, legible mechanical drawing, including pin positions, required hole diameters and also showing where metal parts of the component may touch the PCB. The drawing must clearly state if the component is seen from the component side or from the solder side.
  • Sufficient information to be able to draw a schematic symbol for the component.
  • Preferably complete manufacturer name and type number for use with the final parts list and as a reference in my component library.
If handwritten documentation is supplied, please be very careful about the typing; errors at this stage may flow through the entire design.
Mechanical specification for PCB
The specification can be a drawing of the PCB or a drawing of the mechanical parts where the PCB is to be installed.
This must include information on:
  • Maximum component height.
  • Areas of the PCB with restricted component height.
  • Location and orientation of mechanical components like connectors, potmeters, switches, displays, mounting holes and test points.
Unless otherwise stated, I will assume that the drawing is viewed from the component side of the PCB.
If handwritten documentation is supplied, please be very careful about the typing; errors at this stage may flow through the entire design.
Component loader restrictions
This can be information on minimum component spacing, component grid lines and fixture requirements.
Soldering machine restrictions
This can be information on fixture requirements and additional support points or holes.
Manufacturer logo and type number
The manufacturer's logo and type number can be on the PCB and on all documentation resulting from the PCB lay-out.
If there can be any doubt about the type number at the time of PCB lay-out, choose a long type number initially; changing a type number from "XX1000" to "YY1" in the middle of a crowded PCB is always possible, while changing from "YY1" to "XX1000" may require component relocation and rerouting around the type number.
PCB version numbers
I use yyww (year, week) as PCB version numbers. If different version numbering is required, please include this information.
Text on PCB
This can be fuse ratings, warnings against high voltages, warnings against high temperatures and test point labels. Although the exact texts may initially be unknown, it is essential to make room for the texts on the PCB.
PCB style specification
This is for products, where the visual impression of the PCB is important, and can contain information on component grid lines, manufacturer logo position, type number position, PCB color, preferred component color etc.
PCB manufacturing information
This includes:
  • PCB material.
  • PCB thickness.
  • Solder mask type and color.
  • Text color.
Gate swapping
To ease the PCB lay-out, I will normally swap identical logical gates or operational amplifiers between the sections within the same package or between packages with the same supply lines to obtain the shortest signal paths and an even distribution of traces across the PCB. Unused gate inputs are normally connected to ground or supply lines while unused gate outputs are left unconnected. If this practice is not valid for a specific circuit design, this must be stated in the supplied documentation. Further gate swapping, like using a spare NOR gate as an inverter, is only done upon agreement.
Ground planes
I will normally add a ground plane to all 'unused' parts of the PCB. If the PCB, or part of it, should not have a ground plane, this must be stated.
If the ground plane should be on the solder side of the PCB (for example to shield between the PCB and other circuits below it) please state this.
With multilayer PCBs, this technique can be used to create an exceptional shielding by placing the ground and supply layers on the PCB's surfaces and the signal layers in between, but such PCBs are extremely expensive to manufacture and it is almost impossible to repair defective signal traces and vias.

Standard documentation for a PCB design

At the successful completion of a PCB design, I will supply the following documentation:
Gerber files
I use Gerber files in RS-274-X format as these have the Gerber aperture information embedded, eliminating the risk of plotting with a wrong Gerber aperture table.
Gerber files are supplied for copper, solder mask, solder paste and component print.
In addition, a copy of the board outline drawing is supplied in Gerber format, but this is normally not photo plotted.
RS-274-X files are in "xx.yyyy" numerical format.
Gerber report files
These are ASCII files with statistical information on the Gerber files for control purposes prior to photo plotting.
Excellon drill file
Control file for automatic PCB drilling machines.
Excellon files are in "xx.yyyy" numerical format, and use the same absolute coordinates as the Gerber files.
Excellon report file
This is an ASCII file with statistical information on the Excellon file and with drill size information.
Component location file
Control file for automatic component loaders and glue dispensers. The file lists the centers and orientation for all components on the PCB.
Schematic diagram, board outline and component lay-out are supplied in HPGL plotter file format. The files use pen 1 only, and are created for use with a 0.2 mm pen.
Manufacturing information
This is an ASCII file with information on the PCB (material, thickness, color, solder mask type and color, text color). The file also lists the filenames used for the Gerber and Excellon files.
Parts list
This is an ASCII file with information on the components used in the PCB.

Additional documentation for a PCB design

Additional documentation for a PCB design can be supplied on request. For example:

Schematic diagram, board outline and component lay-out can be supplied on paper.
AutoCad DXF files
These files are usable for verification of the design in AutoCad and for plotting specific details with AutoCad. They can not be used for further PCB design (although modifications can be made in AutoCad), as the PCAD design hierarchy is flattened out to pure graphical data. A file, documenting the layer structure I use in the PCAD files, is supplied with the DXF files.
A complete setup for loading the Gerber, Excellon and HPGL files into the GC-PREVUE can be supplied. GC-PREVUE is freeware and can be downloaded from GraphiCode, Inc.
Film plots of all relevant files can be supplied, but as most PCB manufacturers need to make their own films to suit their manufacturing equipment, this is a very uncommon request.

Data storage

At completion of a design, the customer will receive - on disks or via e-mail - a complete copy of both PCB manufacturing data and all other relevant files used for the design (not the PCAD programs - sorry). Unless otherwise agreed, I will store copies of the files for 5 years in 2 different locations. I do not store the paper based documentation.

Error sources and unnecessary costs

This section lists some common sources of errors and some other points that will add unnecessary costs to a PCB design.
Customer specific Gerber aperture table
The workload for implementing a customer specific Gerber aperture table is excessive as it requires modification of some 500 apertures and all the parts used in the PCB. I use the RS-274-X file format with its embedded aperture table. Most modern photo plotter software will read these files.
Custom manufacturing file names
This requires renaming of the automatically generated files and modification of my standard documentation.
Change of logo or PCB type number
Requires modification of schematic and PCB databases and creation of new plot files.
Sloppy handwriting
This is one of the most common sources of error in handwritten documentation. It will often pass straight through the PCB design and is only discovered when the PCBs have been made. So PRINT CAREFULLY!
Typing errors
I have no means of discovering typing errors in for example PCB type numbers. So WRITE CAREFULLY!
If you send documentation with small type faces via fax, please enlarge the documents before sending them.
V Line
Product design
PCB lay-out
V Line
Hi-Fi products
PA products
Recording & studio equipment
Test & measurement equipment

Poul Petersen, C/Faya 14, 35120 Arguineguín, Las Palmas, Spain.
Tel/Fax: (+34) 928 152 807, Skype: poul.petersen.gc.
http://www.poulpetersen.dk, E-mail: pp@poulpetersen.dk
Copyright © Poul Petersen 1998 - 2015. Valid HTML 4.0!