www.eda.co.uk

This TechWatch is based on the third section of my "I didn't know you could do that in Altium Designer 6" presentation at our user conference on the 31st October 2006. This section covers hints tips and tricks within the Altium Designer Board Level Environment.  Previous sections, Part 1 & 2 covered the Altium Designer Environment and Parts 3 and 4 covered the Altium Designer Schematic Environment.

Each section is divided into parts, in Part 5 I will cover the hints and tips shown for PCB Editing and Selection under the Board Level Environment section.

The Board Level Environment

Within the Altium Designer Board Level Environment we looked at hints and tips for PCB  Editing and Selection, Board Insight Display and Cross Editor Navigation/Selection.  Under PCB Editing and Selection we looked at the New Selection Tools, Routing Track and Via Sizes, and Fanout of BGA's.  With Board Insight Display and Cross Editor Navigation/Selection we explored the many different ways of displaying and interrogating information on the PCB and cross probing between the Schematic and PCB editors, see Part 6.

PCB Editing and Selection

New Selection Tools

There are two new selection tools available to us in PCB with AD6.  They are Touching Rectangle and Touching line which can both be found under the Edit » Select Menu.  These tools will select objects which touch the lines of the rectangle or line you draw, previous selection tools will only select objects contained completely within the rectangle.  A useful tip here is to use the Ctrl Key while selecting with these tools if you want to ensure you do not select any components.  For example selecting Component Pads to perform Multiple Trace routing.

1. Using the Edit » Select » Touching Line (S,L).
2. Hold down the Ctrl key and then Left Mouse Button Click to draw the selection line over your desired Pads.

You can now use the Place » Multiple Tracks to route all of these pads at once. For more information and take a look at this Demo Video from Altium PCB Selection Tools

Routing track and via sizes

There have been some enhancements to the Interactive Routing tools which allow you to setup favourite track width and Via sizes. Under Tools » Preferences » PCB Editor » Interactive Routing we have two buttons to setup Favourite Interactive Routing Widths and Via Sizes.

Within the resulting dialog boxes we can Add, Remove and Edit our favourite widths and via sizes for both Imperial and Metric.  Once these are setup, while routing (Place » Interactive Routing), you can use the short cut keys Shift + W or Shift + V to bring up the favourites selection dialogs and select your Width or Via sizes respectively.  Note these favourites will not allow you to break your Routing Width and Via Design Rules.

Another useful tip for changing Widths while routing.  If you start routing a track, hover your mouse over another existing track on the board of a different width, Press Insert and it will clone that track width to your current track placement. 

To bring up a list of shortcut keys whilst in a command you can use Shift + F1, this will produce a menu style list of you short cut keys at your cursor.  On a UK keyboard you can also use the @ key.

Fanout of BGA's 

An enhancement to the fanout capabilities of AD6 allows you to not only fanout your footprints as before but on a BGA it will also allow you to include escape routing.  Using the command Auto Route » Fanout » Component we now get a dialog box asking to include pads without nets, escape routing and the option to fanout the outer two rows of pads.

Go to Part 6 or back to Part 1.