Engineering and Technical Support Group
School of Information Technology & Electrical Engineering

PCB Dimensions

Absolute maximum PCB dimensions = 230mm x 150mm (9.05 inches x 5.90 inches)


Design Rules > Routing

Protel 99 Path = Design > Rules > Routing

> Clearance Constraint

= Polygons, pads, vias & general clearances must be configured

Name

Optional

 

Optional

 

Optional

Scope 1

Polygon

 

Pads, Vias

 

Board

Scope 2

Board

 

Board

 

Board

Connectivity

Different Nets

 

Different Nets

 

Different Nets

Clearance

15mil

10mil

12mil

08mil

05mil

Remarks

Preferred

Absolute Minimum

Preferred

Absolute Minimum

Absolute Minimum

> Routing Via Style

= 50mil dia / 20mil hole

= 30mil dia / 12mil hole

: Preferred Size

: Absolute Minimum

> Width Constraint

= 06mil to 10mil

= 04mil

= xxmil

: Preferred Minimum Size

: Absolute Minimum

: User Defined Maximum


Design Rules > Manufacturing

Protel 99 Path = Design > Rules > Manufacturing

> Hole Size Constraint

= 12mil (0.3mm)

= xxmil

: Absolute Minimum

: User Defined Maximum

> Hole Size Increments

= 4mil (0.1mm)

: Workshop Requirement

> Polygon Connect Style

= Rule Attributes

= Conductor Width

= Conductors

= Angle

= Filter Kind

= Pwr Plane Clearance

= Relief Connect

= 10mil

= 4

= 90 Angle

= Whole Board

= 15mil

: Nominal

: Nominal

: Nominal

: Nominal

: Nominal

: Nominal


Position in Workspace

Place the PCB design such that the lower left corner of the PCB is at workspace coordinate 1000mil, 1000mil.
 

Borders

  • Ensure borders are created on ALL electrical layers using 10mil tracks.  We require these borders to assist in artwork alignment (Tip - try using Multilayer for borders).
  • It is recommended that there is a minimum clearance of 120mil (3mm) between the edge of the board and all PCB elements.
     

Mounting Requirements

  • Do you need mounting holes
  • For M3 mounting holes use PCB library component SPACER01 in KBpcb05 library
     

Final Checks

Ensure you check your schematic running ERC, and PCB by running DRC

 

Libraries

It is important to note that a large number of PCB footprints intended for through hole components supplied by Protel/Altium are incompatible with our manufacturing process.

It is therefore recommended that you use the Electronics Engineering Laboratory Libraries which support many of the components held by this facility and are fully compatible with our PCB manufacturing process.

Schematic and PCB libraries are available for download from the Engineering & Technical Support Group website.

If you have already designed your PCB using (TH) footprints supplied by Protel/Altium, it is suggested that you carry out a thorough inspection with respect to physical size, annular ring and hole size requirements for each component before submitting your design for manufacture.

Library Catalogue Access

The Protel/Altium Library Catalogue displays the contents of our Schematic and PCB Libraries and is accessible at the following locations:

  1. Electronics Engineering Lab student computing area  >  Non-removable hard copy
  2. Engineering & Technical Support Group website  >  PDF/ZIP files for download

Feedback

Please email any suggestions to the Engineering & Technical Support Group Manager