May be a problem is with my English but for me it looks like red are at front and green are at front.
When designing PCB I look into schematic only during first phase - sorting footprints into groups according to schematic. Then I close schematic and work only at PCB so any colors at schematic would not help me.
To help in remembering what way I am planning to route the track I sometimes route part of it temporarily just to make connection lines be positioned where it will be probably routed.
It sound like you want or expect eeschema to realize the entire flow rather than appreciating that it is one viewport of the overall design you are trying to realize.
The schematic capture is one viewport, the pcb layout is another, gerber is another, the BOM is another, each providing a different way to look at the solution that offers insight.
When a circuit is captured there are certain conventions because it is a visual representation of the intent. A well drawn circuit clearly shows the intent: Low pass filter here, inverting gain there etc… This enables the bigger picture of intended functionality to be visualized quickly and concisely ( A poorly drawn circuit adds ambiguity or you lose focus of the bigger need… I reviewed someone circuit 15years ago and on an A3 page the feedback resistor of an OPAMP was the other end of the page and the entire circuit was a ratsnest of nodes…
At this stage you don’t really care whether a component is top or bottom side, whether the PCB is 2,8,16 layers. You might however start having an idea about critical paths and thus might place notes on the circuit (keep loop small on a SMPS, track as a diff-pair etc…). Likewise a few rules of thumb would already have you settling on 2,4,6 etc layers and the type of stackup.
In the PCB view its more of physical connectivity and the focus is more on manufacturability and physical effects (heating, pickup, radiated etc). Placement is an important step to keep functionality close and placed in a logical positions to optimise the flow. you might get everything on one layer but that wastes space. You place things on the other layer you obviously need a via to change layers. These do not need to be captured in the schematic view as it clutters such a view and does not bring any benefit especially for something like a via or the layer of a part.
The BOM view can help rationalize the type of components. More often than not when I am capturing a circuit I am re-using or I get tunnel vision with the problem and chuck a 100nF to complete the view. When I look at the BOM and see I have 10 different 100nF that’s when I go “ooooh” and start changing them all to the same type (or minimize the number due to voltage considerations)
Having PCBnew and EEschema open at the same time to permit cross-probing is key here because if you just look at the layout you can lose sight of the function while also viewing it in the circuit viewport provides that additional information and thus permitting compromises in key area’s. Take a SMPS… I would ensure the main switching loop is as small as possible to stop EMI issue and equally the feedback is routed to ensure a “clean signal”. Does this mean that the soft-start caps or UVLO needs to be placed elsewhere routed using via’s? sure and at this point I might decide to add an extra capacitor to help alleviate some potential noise problems
remember… Engineering is all about compromise
Everyone has their own style of drawing a schematic but instead of using a line (wire) to connect components labels are often used. The name given to a label can add more meaning than just a line and it reduces clutter on the schematic. It also helps in PCBNew when nets have more meaningful names.
I’m wondering why, at this stage, you even care what is on the front vs back? What are you trying to achieve by deciding what should be on the front vs back? The schematic is the design of the electrical circuit(s). It is the place for defining such things as the values of components such as capacitors, resistors and ICs, as well as how they are to be connected. The schematic does (should?) not define such things as the number of layers or if the components should be SMD or through-hole, etc. The same schematic could then be used to route a single sided board, a two (or more) layer board or even hand wired on a perf. board or prototyped on breadboard. For more complex designs the schematic may include notes that aid in board layout such as target impedances, groups of signals that should have the same trace length and how that group relates to other groups, current carrying capacity of a trace, etc.
Another angle to consider: What if you have to adjust the design to accommodate changes - i.e., changing an SMT resistor with a higher-wattage resistor or even just adding / removing parts from the design?
When working with multi-section ICs (74xx or dual / quad op-amps), it sometimes happens that swapping sections on the schematic will help make the routing go easier.
Focus on making sure the schematic is correct and the proper footprints are in place, then focus on the physical layout of the parts on the board, make sure the assignment of multi-section parts works well, THEN you can worry about the actual trace routing. 
In eschema you can add names to each run. You could simply append a “_R” or “_F” to those connections you wish to be on the front or back.
The other thing I think is important, have a printed copy of your schematic as you are laying out the board. As I am designing a circuit, the component numbers are meaning less because I will reannotate the schematic when completed. So I find it easier to have a printed schematic as I layout the board.
If you watch this silent video you can see why you are wrong [ by silent I mean the soundtrack conveys no useful information about the circuit ].
The only requirement for the finished circuit to work properly is that the nets shown on the schematic connect ONLY at the red dots shown on the schematic.
Creating a two-dimensional surface is only used because
Imagine if you pick up the circuit shown in the video. Will it still work? Yes, if you pick it up with dry hands or hands wearing dry plastic gloves. On the other hand, if you pick it up with a pair of metal alligator clips, you will probably short out nets that aren’t designed to be shorted out. This is true whether the circuit is flat or shaped into a ball.
So… What color should ^^^those^^^ “wires” be in Eeschema?
I think the key here is to remember the workflow for a project.
The important point is that the choice of layer for a wire is done at step 10. If the board you are designing becomes to complicated or the signals are noisy and you need more separation/ground planes — it’s relatively simple — visit step 6 and increase the number of layers. Then select the wires for the the new layers.
No need to alter the schematic - which becomes part of the documentation.
Warning - if you add a run using PCBnew which doesn’t exist on the schematic – you’ve got a problem. If you correct the schematic and update the PCB from the schematic - that manually added run will disappear.
If you follow the work flow sequence, eschema, simulate, foot prints, BOM, PCBnew, you also have the opportunity to use KiCAD to create a 3D view of your board.
If you want mounting holes on your board - they need to be on the schematic !!! They are imported from the schematic into the PCB layout the same way as the other parts!
If you want to add additional annotations for parts - you do that on the schematic — and update the PCB board from the schematic. Remember the workflow!
If you jump out of sequence on the workflow - it creates rework.
On the far right of your PCBNEW screen, right of the lay tracks and other buttons that control what you draw, is a column of colored squares. These are labeled as the last thing on the right. Do you need to scroll there? F.Cu is front copper layer, B.Cu is back copper layers. F.Silks is checked if you are putting writing on the front of the board. Edge cuts is the outer edge of the board. Just click layer you want do something on. If you hadn’t discovered this column, KiCad is way better than you thought!
This may be hidden:
On V5.1.x
View - Show layers Manager
On V5.99
View - Show Appearance Manager
This topic was automatically closed 90 days after the last reply. New replies are no longer allowed.