I need to design a PCB layout to a system using an isolated communication with optocouplers, what means that I need separated ground areas, each one on one side of the communication that I want to isolate. So, is that possible to do it? How could I do it in a simple way?
You can solve your problem using the ground terminal in both sides of your schematic as the image below.
The point is that in the layout process you have to draw two different ground areas and just ignore the link between them as is shown in the image below.
You should not call both of them "ground" if they are isolated from each other. Create the second one as its own net with a different name. Vss is a popular choice.
As for with the LM319, two GNDs are separate - for example, pin 6 and 8.
@borges: "Just ignore the link between them" ? Terrible idea. If you're going to bother using a PCB design package at all, why design your circuit such that fundamental Design Rule Checks can't be used at all? That's the whole point of these programs!
@OP In ISIS / schematic layout (depending on Proteus version) go to Tools -> Configure Power Rails. From here you can create a zero-volt power rail and name it something suitable.
It is common practice to have different visual symbols for separate grounds, which removes ambiguity when reading the schematic, but you need to know how to create your own symbols first. If it's just you reading the schematic you can probably survive fine using the standard POWER symbols and naming them differently. Proteus comes with GND and CHASSIS power pins by default; there's nothing stopping you adding a new entry to the list.
However, you MUST pay attention to hidden pins in IC circuit symbols. A typical logic IC, let's say a 4001 or a PIC, will hide it's power supply pins from the schematic to save unnecessary clutter. You need to edit the properties of any such component and find the Hidden Pins button (top right hand side of properties window) and make sure the supply pins go to the right nets.