Here goes. PCBs are made up of a series of layers. For a single sided PCB, you will have your copper on the bottom together with a solder mask. the solder mask is the green laminate that they put over PCB tracks to stop the solder flowing all over the PCB tracks. Obviously you want to keep the PCB pads exposed so they can be soldered to.
Also for a single sided PCB, you will have a silkscreen on the top layer that shows the outlines of all your components. This is just another layer of the PCB and you have to tell the PCB maker that you want this as silkscreen and not copper (see below). Seetrax recommend that you have your component outlines on layer 3 and your text on layer 4. You then go on to specify (see below) that you want these layers as silkscreen.
With a 2 sided PCB, you will also have a top layer of copper (track on the top of the PCB). This can be added as an extra layer. If this is the case, once you have designed your PCB, you need to specify that you want your top tracks as copper.
Vias are plated holes that are drilled through the PCB. They link the top layer of the PCB with the bottom layer. If you have a single sided PCB then you will not need vias.
Below are some notes I made for myself years ago when making PCBs. It is also probably best if you phone Seetrax and ask them to send you a pdf of the instructions. I have a copy on my PC, but am not sure about copyright etc. They are very helpful
The notes below apply once you have laid out your PCB
Creating Outputs:
Set data format to Excellon
Set Units to Inches
Save Drill Data
Save Rout Data
Save Tool Data
Saving Gerbers in Olimex format:
Select Photoplotter -> Setup -> auto job dcode table – Go into Properties and Selected dCodes as extended Gerber
Select Solder Mask -> Setup
In Setup
Set pad swell to 0.015”
Set X shift to 1.000
Set Y shift to 1.000
Tick Plot Profile box to define edge of board
Tick Plot Target box
Tick ‘Include Vias’ Box if you have used Vias or wire links
In Layers Selection
For Bottom Solder Mask:
Select what you DO NOT want covering
Tick Bottom + Pads only (to stop them being masked)
Tick V + Pads if vias and wire links are included
Close dialogue box
Do Plot Preview (next to GO button)
Hit the GO Button
Save file as Bottom Solder Mask.ger
For Top Solder Mask – only if you have tracks on the top layer. If you have vias and you print a top layer, you will get solder pads on the top layer:
Select what you DO NOT want covering
Tick Top + Pads only (to stop them being masked)
Tick V + Pads if vias and wire links are included
Close dialogue box
Do Plot Preview (next to GO button)
Hit the GO Button
Save file as Top Solder Mask.ger
Select Artwork Layers -> Setup
Select Plot Targets box
Select Plot Profile box
DO NOT select Plot Keepouts or your keepouts will come out as copper
In Layers, select Bottom Layer: Pads and Copper
Select V layer Pads if you have wire links or vias
Do Plot Preview
Hit the GO Button
Save file as Bottom Copper.ger
If you have tracks on the top layer:
In Layers, select Top Layer: Pads and Copper
Select V layer Pads if you have wire links or vias
Do Plot Preview
Hit the GO Button
Save file as Top Copper.ger
Select Artwork Layers -> Setup
In Layers, select Layers 3 & 4: Pads and Copper
Include Layer ‘T’ Copper if you have wire links – this will treat all artwork on the top layer as Silkscreen, not copper
Do Plot Preview
Hit the GO Button
Save file as Top Silkscreen.ger