Layers in CADSTAR.

As requested - some information on setting up your layers in CADSTAR.

(Pull up a chair and make a coffee - its a long one).

What is all this layer stuff about then?...

So you are designing a printed circuit board - this is generally a fibreglass inner core with copper tracks on the outside. Although the inner core can be made of many different laminate materials depending upon the boards use, FR4 (Fibreglass) is the most common.

On the outside copper layers, which are completely covered in copper before the board is made - the tracks that you design will be what is left on the board when it is manufactured.



Because PCBs are getting more and more complicated we need more tracks than we can have on the outside layers alone. As such we can also have inner layers of copper that can be used for tracks.

Boards will generally go up in pairs of layers, 1, 2, 4, 6, 8, 10, 12 and so on. If you consider that your computer motherboard can have between 12-20 layers we need to setup a layer structure in CADSTAR to reflect what the actual board will look like so that we can design it correctly.

Have a look at this standard build and I will try and explain how you might recreate this 6 layer board in CADSTAR.

From this you can see that we have outer and inner copper layers - these are for the tracks that make up your circuit. Also we have some laminate cores -these make the board the required thickness with rigidity and strength. Additionally between copper cores we also have what is called pre-preg this is pre impregnated insulating material. All the layers are placed together and pressed under very high pressure to make your board.

So how do we do this in CADSTAR?

First you need to consider the technology used in the design. If it is not high speed and you are not using impedance matching etc then you do not need to be defining the inner cores and prepreg for anything other than making it look like a real board in the layer picture. We only need the copper layers.

To setup your layers in CADSTAR, from the menu choose Settings\Layers.
This brings up the following screen:

(Click on the image to view it larger - hit back to return to this page)

In CADSTAR there is a Physical layer and a Logical layer.

Physical layers correspond to the sides of the laminate and are numbered 1, 2, 3, 4, etc.

Logical Layers correspond to the layers on which you design your PCB layout. These Logical Layers are of different "types" so that you can create them for specific purposes (i.e.. Electrical, Non-Electrical, Documentation, Power Plane, and Construction). You name these layers to indicate their purpose (e.g. Solder Resist, Silk Screen, Component).

Each Physical Layer may require several Logical layers. For example, Physical Layer 1 (Top Elec) may require the Top Elec/Copper, Silk Screen layer, Component layer and the Solder Resist layer to complete its manufacture. So the relationship is many Logical Layers to one Physical layer:

In the example above the Minimum Physical layer is 1 (Top), and the Maximum Physical layer is 4 (Bottom).

Given that when we are looking at the board on screen we are looking at the top layer closest to us, making it the minimum, through to the bottom side being furthest from us so it is maximum.

So to return to our 6 layer board, we have the maximum physical layers set to 6, we have 6 electrical (copper) layers numbered 1 to 6 and for sake of the visual effect we add some laminate layer in between.

For our power and ground connections we would generally designate an entire layer for each connection so we have one for VCC (the powerplane) and one for GND (the Groundplane), each copper layer is completely covered with copper and in CADSTAR they are both referred to as a powerplane.
So now we change layers 2 and 5 to powerplanes. When we change them to a powerplane, in order to create an association to the electrical net that the layer is used for we name the layer the same as the net name. This way all GND connections will connect to the GND powerplane automatically & so on for the VCC layer.

On the outside of our board we have other layers such as silkscreen, solder resist etc, these are all "non electrical" layers (as they are not used for anything electrical like tracks).

Each component (footprint) will have various features on each of the non electrical layers, silkscreen outlines on the silkscreen layer, placement courtyard outlines on the placement layer.

CADSTAR supports the ability to create different sized pads on different layers so that we can make our manufacturing files exactly how we want them - so this is why we have solder resist and solder paste layers either side.

Each layer is created, named and given a description. The type of layer is chosen, Electrical for copper layers, non electrical for the non electrical features, powerplane for the power rail layers, Construction for the laminate/prepreg layers and Documentation for any other layer that contains documentation items or perhaps only figures/text/shapes etc.

For the non electrical layers, if you are going to be outputting ODB++ or interacting with a 3D modelling program then we need to be able to tell the software exactly what the layer is used for (in addition to the name) as a class of layer - this is known as the "Sub Type". I.E. the Top Silkscreen is  "Silkscreen" Sub-Type.

The physical layers have already been explained - however only the outside copper layers will have non electrical layers assigned to them using the same physical layer number.

Then you have the "swap layer", this allows component items on one side of the board to be mirrored to the other side. I.E. the Top Copper will swap to the Bottom Copper, and so the Top Silk will swap to the Bottom Silk. I cannot see any sense in swapping them to any layer other than the identical opposite one.

For the electrical layers you can then setup a routing bias, this is to say that the tracks on that layer when added by the auto router will follow the direction that you set. It has been common for tracks on one side to go in the X direction and tracks on the other side to go in the Y direction. This is down to personal preference and does not have to be adhered to but is recommended for a good layout with least problems.
(although you can use common sense and go in any direction when manually routing the board).

Obstacle specifies that a layer with this type of bias is a non-routing layer, which contains obstacles which must be avoided when vias are inserted.

Then you have the thickness, this is how thick that individual layer is. I.E. a 1oz copper layer will be entered as 33um or 0.033mm, although the copper may actually be half that and plated during manufacture to bring it to 1oz.
After giving the electrical layers some thickness's, the construction laminate layers are given thickness's to bring the board to its final overall thickness (I.E. 1.6m).

The Material column is where you tell CADSTAR what materials the layer is made of, I.E. the Construction Laminate core is FR4, the copper layers are "Copper Film", the pre-preg layers the particular pre-preg used. Each type of material can be added using the "Materials" button where you also include the permittivity of each material (see your board manufacturer for this information).

Embedding is specified for Electrical  layers only. You would not normally specify embedding for Power Plane layers.

This parameter specifies how an Electrical layer embeds into a softer Construction layer (e.g. Prepreg). It can be either Above, Below. or None.

Above specifies that the copper projects upwards into the Prepreg
Below specifies that the copper projects downwards into the Prepreg
None specifies that no embedding takes place.

Note that the outer Electrical layers do not have embedding specified - that is because they embed into air, not into a softer Construction layer.




Now after writing all the above I think I need a rest so It's time to say - For further information about the layers please consult the help file.