You may have heard of manufacturers referring to the piece of substrate used to create pcbs as a panel.  In essence, panels in Easy-PC are a way of assembling multiple pcbs together in one place in a similar fashion.  Panels can be created manually or by using a wizard.  Note that embedded designs are not WYSIWYG.  Silk and board information is displayed for orientation but most data is omitted.


The most important precondition for panels is that all the pcbs embedded in them must have the same number of electrical layers.  There is some flexibility for non-electrical layers, but the electrical ones must correspond.  You can't combine 2 and 4 layer designs in the same panel.

To start a new panel, go to [File], [New].  You can either use the [Design] tab if you are confident about how to do this, or the [Wizard] tab for step by step guidance.  In both cases select the [Panel Design] entry.

Wizard tab

At any point press <F1> for more help with the current screen.  The [Wizard] option allows you to choose a technology file, otherwise the layer stack of the first design added is used.  The program remembers the last design used and will offer this, but it's also possible to browse to any different design as required.  If you are warned that the stored design is no longer available, just click through the message and reselect.

In the next screen, non-electrical layers will, as far as possible, map automatically to matching panel layers, but where there's a mismatch, it's still possible to complete the process manually.  Here you also choose whether to use a fixed or a relative path to the embedded design.  If you choose a relative path you will have to save the panel design in the last step to establish a baseline, but a fixed path can be less portable.

Following this, you define the size of panel required.  The next screen allows you to set up step and repeat parameters for the chosen design but can be set to one iteration if a mixed panel is planned. Finally, you are prompted for a panel name and can opt to save the panel.  Whether saved or not, it still opens in an edit tab for further work if required.  For details of this, see the next section.

Design tab

For the [Design] tab, remember to choose an appropriate technology file, bearing in mind that the electrical layer count must match the designs.  The layer content can be edited after creation in the same way as for pcb designs if required.  Once [OK] is pressed, the new panel opens in a fresh tab with a default name.  If embedded designs are to use a relative path, this panel will need to be saved to file to establish a baseline location.

To add a design to the panel, use [Add], [PCB Design].  If the electrical layers do not match, you will be warned that it cannot be added. If the layers do match, the add design dialogue for the previous addition will appear, allowing you to browse for the next design to be added.  Once this has been defined, you can adjust any layer matches as required before accepting the design.


Any embedded design can be repositioned, rotated and fixed in much the same way as a component in a normal pcb design.  Many of the usual items can be added as with a pcb - text for labelling, shapes for adding scoring lines, for example, pads and components for possible fiducial markers.  The full list is on the [Add] menu.


The usual plotting dialogue is used for output, but there is a difference.  For each of the plots, there is a new 'panel' section on the 'Settings' tab, with two entries.  The first is straighforward - just including any panel outlines in the same way as board outlines for a pcb design.  The second is critical, and must be enabled to include the contents of the embedded pcb designs in the output plots.  Failing to check this box for every plot is the commonest problem with using panel designs.  If you use panels regularly, you may wish to save a fresh set of settings after this has been enabled for each plot.