Skip to main content
shopping_basket Basket 0
Login

The mysteries of the PCB board outline

0

Foreword.

DesignSpark PCB users often raise interesting questions with our support team, one recent example is

"What defines the board edge dimensions since the outline has a thickness?". 

The simple answer, "It is the centre line (not the inner or outer edge)".

For most users this is all you need to know, so feel free to leave now and get on with your PCB design and use the default settings, but do check you meet your board manufacturers requirements before producing and submitting your Gerber plot files.

For our users who would like a more in-depth discussion, please 'read on'.

What thickness or style for the board outline should I use?

Where is the actual machined edge going to be?

For this discussion we will start at the end! 

CHECK with your manufacturer where they will mill the edge of the board to in relation to the board outline line width.

Many clearly state they mill to the centre of the board outline line width but you need to check as you will see below, it's not always clearly stated.

Some typical extracts from websites:

  • "The tool that routes the edge of the board cuts up to the middle of the line."
  • "Make the outline trace thin 0.1Mil or less. This way there is no ambiguity as to which edge of the line is the intended edge of the boards."
  • "We recommend a small but nonzero line width; the fab will route so the edge of your board is at the center of your line, no matter how wide it is."

DesignSpark PCB and Pro define the board size to the centre of the line style used. The default line style of 5 mil is used which is good for screen visibility and suitable for manufacture, but you can change this to meet the manufactures specific suggestion.

board outline

DesignSpark PCB and Pro both use the line style width for the purposes of the Design Rule Check calculations and also for the copper pour gap.

This means the inside edge of the board outline is used for these calculations, this is not an error as explained below.

board to copper gap

It can even be considered an advantage and be used to indicate the width of the machining tolerance while designing the board, and then the width reduced to the manufacturer's suggested line width prior to generating the Gerber plots.

The image below illustrates that the centreline of the board outline will be used to indicate the board edge, but there is also a machining tolerance when the outline is milled and this is shown by blue dotted lines.

If the precise size of the board is very important check with your manufacturer.  Typically, the board outline will be milled to +/- 8 to 10 mil as standard or +/-5 mil as a custom requirement from the board outline centre line. For this reason you may wish to increase the board outline line width to 16 to 20 mil to show the possible final size of the PCB, but do ensure you reduce the line width to the manufacturers recommend value (if specified) before generating your Gerber plots.

Please always consult with your PCB manufacturer as to how they will produce the board, requirements and rules vary from manufacturer to manufacturer. 

Note. The line widths in the images have been made larger than normal to illustrate the issue.

board machining tolerances

There are two methods of including the board outline within the Gerber plot files as described in this article "How can I add a Board Outline to my Gerber Plots?"

The simplest method detailed adds the board outline to the "top copper" plot...

Now you will understand why the inside edge of the board outline is used for the copper pour gap as there could be a fine copper trace around the edge of the board! 

The copper pour in this instance keeps the correct gap as defined in the Design Technology - under "Spacings". You may wish to set this spacing slightly larger to account for the board outline machining tolerances and the board outline.

spacings table

If you are concerned about having copper around the board edge use the second method in the above article and create a Board Outline Gerber plot.

Manufacturers may also remove the board outline from the copper layer before processing, but this again is manufacturer specific.

Recommendations and Conclusion.

1. Please always consult with your PCB manufacturer how they will produce the board, because requirements and rules vary from manufacturer to manufacturer.

2. Select a PCB board outline width of 5 mil or less as recommended by the manufacturer. This will probably meet most user requirements.

3. Decide if milling the board size to the centre line or inner edge of the board outline is important, if it is then check and meet the manufacturers requirements.

4. There is also a machining tolerance to account for if the final board size is critical.

5. Remember the above is discussing minor issues of a few mil...

RS Components / Allied Electronics Support for DesignSpark PCB

Recommended Articles

DesignSpark Electrical Logolinkedin