Sometimes it's necessary to separate low current and high current areas within the same net, as voltage drops in the high current areas could have an adverse impact.  The usual approach to achieving this is to kep the low and high current areas independent of each other, connecting them at a single point, commonly known as a star point.  Easy-PC regards all connected points as at equipotential within a net, so the simplest way to achieve the necessary isolation is to use two different nets, which works well, until they're joined and become one net.  To vercome this, any pad may be designated as a star point, allowing pads so designated to be overlaid without generating pad to pad errors.


Before covering this in detail, within the program there is more available on this topic under [Help], [Contents], [Index] tab, under the [Star Point] entry..
There are two broad approaches to this.  Either free pads can be designated as star points, or components containing the necessary structures can be used.  The difficulty with free pads is that no schematic equivalent exists.  There's no obvious way to designate the two nets so it's clear they are common, which only leaves one solution.  That is to link the two separate nets, not with a connection, but with a line so that the nets will not be joined, but in any printout of the schematic, it will be clear that they are linked.  As described in the help article, both pcb pads must be perfectly aligned (which can be checked and adjusted if necessary in the pad properties) and no more than one can have a drill hole.  Joining nets in this way is not restricted to two.  As many pads as desired can be stacked above each other as long as all are designated as star points and perfectly aligned.
Moving on to components, the help describes how to use components containing a single star point, but this is not the only way to approach this.  We will consider a two star point component, though this can be expanded to the required number using the same techniques.  In the schematic symbol, placed two pads separated by one grid step.  Add a line (not a connection) between them.  When connected, these pads will apparently merge into the nets.  Disable pin names and numbers for both pads, and don't add a reference origin.  The symbol can now be saved.  For the pcb symbol, define two identical pad styles, but with one hole set to zero size.  The other should be an appropriate size for a via or component leg.  Align these over each other.  Again, no reference should be placed and pin names and numbers disabled.  It's possible to sve the symbol at this point, but you should also consider whether to add two short single lines using a style the same as your usual track width, one in each direction out of the pads.  They need to clear the pad by at least the normal track to pad spacing.  In the properties of each copper stub, link one to each pad, so each pad has a stub associated with it.  Do not enable the 'Auto Mask' feature.  This alternative symbol can now be saved.  Why two symbols?  It's to do with design rule errors.  The pad to pad and pad to track errors are suppresed, but track to track are not, so connecting directly to the pads does result in track to track errors.  If the tracks are stopped short over the stub copper, these errors do not occur, but the tracks will be flagged as dangling.  However, a connectivity check will show that the net is complete as the program recognises the overlay as a valid connection.  The downside is that as the tracks don't terminate on the pads, each pad will need to be added to the appropriate net.  It's your choice which approach is the least intrusive.  Remember that stubs can also be used if desired with the single star point components described in Help.  In this case, use rotation to separate the stubs from each other.  When creating multi-pin star point components, use [Edit], [Assign pins 1:1] on the pin assignments tab to link the symbols.
Whichever approach is taken, to make selection easier, either use the ext hotkey for the next item within picking range, or hold down Alt> before left clicking to open a mini menu of items available for selection.