How to use the copper pour dialog.

New and improved copper pour functionality has been added to DesignSpark PCB with the release of V8.1.

The new functionality has required a redesign of the tool window as detailed below.

For single or multiple copper pours with the same settings, the defaults applied are initially loaded  from the shared settings for power planes and copper pours from the Design Technology - "Rules" tab.

These settings will be used for any copper pour on your PCB unless overridden. Individual copper pour areas can be customised on the PCB using the copper pour "Properties" prior to the pouring function.

Due to the increase in options available they are no longer part of the copper pour window as in previous versions.

Copper Pour Properties.

Select the copper pour by a left mouse click on the copper pour boundary, then right click and select "Properties". The properties window now displays, select the "Area" tab.

The yellow highlighted area shows the values populated from the Design Technology "Rules" and these will be applied to this selected copper pour area.

Previously available features such as setting the copper pour "order" and the option to set this area as a "Keepout" are still available.

"Help" within DesignSpark PCB provides details of all the features.
Using the the index "Copper Pour Area Properties" provides a good overview, however all topics related to "copper pour" should be referenced for specific details.

A summary of the features is provided below.

If the settings for the selected copper pour area require to be changed, select the check box "Override Design-Level Thermals". From the pull down menu select to change the values that will be applied individually to through hole pads, surface mount pads and vias.

Having selected what you wish to override, now select the available options by selecting the "Override Default" check box and selecting from the pull down list.

For each option in the list the settings can be changed in the value boxes, only values appropriate to the item are in bold and can be edited. Here "Orthogonal Spokes" shows all the values can be overridden.

A description of the options:

• Orthogonal and Angled Spokes - these will be generated with the aim of producing selected number of spokes, success will be if at least the minimum spokes can be achieved. If this is not possible then the pad will become isolated. Always check for isolated pads!
• "Preferred" Orthogonal and Angled Spokes means try to add at least the minimum number of spokes using the preferred style, otherwise change to a different style (angled or orthogonal) to achieve the minimum. If the minimum cannot be achieved the pad will become isolated.
• Isolated from plane - will allow a pad e.g. on the GND net not to connect to the GND copper pour. This allows specific signal or grounding requirements to be achieved.
• Not isolated (flooded) - the copper pour will flood across a same net pad and it will be lost from view, but in production will be present once drilled.
• Adjacent (touching) - will pour up to the edge of the pad such that you will still see the hole in the view.

The copper pour now provides greater flexibility. Used in conjunction with overlapping pour areas and setting the pour order allows more complex requirements to be achieved.

With this greater flexibility an important point from "Help" is how to reset any custom settings:
"you can 'refresh' the values attached to the area by unchecking and re-checking the Override Design Level Thermals checkbox. This will copy the new values down from design level to this area, ready for you to set your local over-ride values once again. "