What are Mechanical Symbols?

Mechanical Symbols have none, or more Mechanical Pins, Mechanical Pins, do not have Pin Numbers. These will be part of the Board when manufactured but won’t be connected to any of the Nets in the Board. Examples of typical Mechanical Symbols are mounting holes, cut-outs, fiducials, re-usable Board Outlines, and so on.

For the Board in this course, a Mechanical Symbol is created to handle the “bare” Board. This isn’t a requirement for creating a Board in PCB Editor since, for many users, there may be few instances where “generic” board outlines are re-used across multiple designs.

 

Creating a Mechanical Symbol for a Board

A Design Outline needs to be defined as Shape on the Board Geometry / Design_Outline subclass. Design Outline encompasses the entire design, in the case of the course design, and other single board designs, this will be the same as the Board outline. For Flex-Rigid designs, not covered in this course, Zones are used to divide the Design Outline into the flexible and rigid sections.

The Design Outline can be defined by drawing a Shape with co-ordinates, the method used in this course, with the mouse in the canvas, or by importing a DXF file. See this note for more details on DXF import: https://www.parallel-systems.co.uk/wp-content/uploads/2020/02/dxf_import_output.pdf

Since the Design Outline is defined as a Shape, Shape Edit Application Mode can be used to edit the Shape like Chamfering and Rounding corners, and adding Notches.

 

Mounting holes

Any mounting holes can be added by placing Padstacks. These Padstacks will typically have been defined as Mounting holes in the Padstack Editor. This is only the case for a Mechanical Symbol, If you do not make a master board mechanical symbol you can place mounting holes that are defined as Mechanical Symbols. See this notes as an example of a mounting hole definition. Mechanical Fixing Holes – Via Rings (parallel-systems.co.uk)

 

Package and Route Keepins

Typically, components and routing will need to have some space between them and the board outline. PCB Editor has Package and Route Keepin Classes for this purpose. These areas can be drawn with co-ordinates, drawn with a mouse, imported from a DXF file, or “Z-Copied” from an existing object. Use of Z-Copy can be especially useful to create Keepins from complex outlines imported from DXF files.

Note that a PCB Editor Board file can have one, and only one, Package Keepin and one, and only one Route Keepin. For users who want to have different clearances between the layers of the PCB and the Design Outline, a Manufacturing DRC rule can be defined to cater for this. (Not covered on this course). Package and Route Keepouts are used to “fine tune” placement and routing restrictions, and there can be as many of these as required. A Min Height property assigned to a Package Keepout restricts the height of components that can be placed with it.

 

Saving Mechanical Symbols

Saving the Mechanical Symbol will create a “dra” file and a compiled “bsm” file. Again, these would typically be saved in a temporary folder for checking before being moved to any “active” library location. Also, keep the “dra” and “bsm” files together in the same location.

 

What are Master Boards?

Master Boards are user defined starting points for new board designs, or Templates. If a new board design is started with “all defaults”, the Units will be Mils (thousandths of an inch) and all rules, constraints, covered later in the course, will be 5 Mils. A user defined Master Board can contain as little, such as merely units and colours, or as much, “everything” that doesn’t not involve the Logic (netlist) for the board, or anything in between, so that designs have a consistent starting point. Users may have a number of Master Boards with the same settings and different cross-sections for 2, 4, 6 and so, layers.

See this note on Template Boards: User Defined Templates (parallel-systems.co.uk)

Having a Master Board is not a requirement and a new design can be started without one. A Master Board will be saved with a “brd” file extension, a single file.

 

Cross Section Editor

The cross section editor is used to define the layers in the board. Printed circuit boards are a “sandwich” of fibreglass substrates laminated with copper and fillers which have no copper – used to build the board to the required thickness. For a two layer board, “standard” laminated material will be used with a 1.6mm thickness and external copper which will be removed by the etching process to leave the conductive connections. That raw material will then be drilled and plated to form the Vias and complete the connections between the two layers. For a board with more than two layers, the fabricator will use the etching process on a number of laminated sheets, to get the conductive elements, and then drill any holes and plate to form any Vias required at that point. The fabricator will assemble those processed materials with fillers and, potentially drill and plate to form any Vias as the build up of the board progresses before pressing and heating that assembly before any final drilling and plating.

The “default” PCB substrate material is FR-4 but the details of the build up of the material may cause the electrical characteristics to vary and discussion of your requirements with a fabricator can be invaluable in ensuring consistent performance.

Other substrate materials are available for applications that require lower dielectric losses than FR-4 can provide.

 

 

In the Cross Section Editor, layers or layer pairs, can be added, or removed. If required, multiple adjacent dielectric layers may be added to reflect the build up of the board.

All conductive layers in the cross-section, Conductor or Plane, may contain routing and shapes but layers defined as Planes will be ignored by the Auto-router. There won’t be any connections on any layers unless routing, and / or shapes, have been added.

Materials used in the Cross Section Editor are loaded from the materials.dat file. There are a number of cross section materials provided in the default materials.dat file in the installation and materials can be edited by using Setup>Materials from the PCB Editor menu. For the purposes of the course, the provided materials.dat file contains a restricted set of materials.

In the Cross Section Editor, the right pointing triangle in the column heading indicates that there are additional details which are not visible. Double click in the column heading to expand the cells and view the details.

The Signal Integrity section provides characteristic impedance calculations based upon the material parameters for the layers and assumes that any planes that are defined are ideal. The impedance calculation requires that at least one Plane layer is defined in the cross section for reference.

 

All content Copyright 2022 Parallel Systems Ltd.