Layers in Altium PCB footprints

[gyuunyuu1989]

I am trying to get my head around what custom layers need to be added into PCB footprint and understand the meaning of existing layers. I saw a video from Robert that described new layer creation this but don't remember which video it was. So basically when we create a PCB footprint, we get certain layers present inside it by default. These are top layer (copper), bottom layer (copper), overlay (silk screen), solder paste, solder mask, drill drawing, drill guide, keep out layer and multi-layer.

From this I get these questions:
1. What is difference between drill drawing and drill guide? I would except this to be used in some way for vias and through hole pads but don't know how. I would expect there to be just one layer called "drill" which contains information about holes and slots.
2. What is purpose of keep out layer? I mean we already have so many other layers like top and bottom copper, solder mask e.t.c, so why do we even need a "keep out layer"?
3. Why do we need something called "multi-layer"? I mean we already have so many layers so things go on separate layers already, so having "multi-layer" layer does not make sense.

Now, lets talk about the custom layers. From what I remember from Robert's, we need to have Mechanical layers which contain this information:
1. 3D Body, this layer had purple color
2. Assembly drawing symbol with designator in middle, this layer had purple color
3. Component boundary, this layer had green color

I have a few questions about this so the first question is, why do we need the green layer when we already have a "keep out" layer that is created by default? I am confused between the concept of "Courtyard" layer and "Assembly" layer. Altium does not name anything as "Courtyard" layer or "Assembly" layer by itself.

[robertferanec]

1) when you start using uVIAs, blind VIAs, buried VIAs, through hole VIAs, drilling becomes complicated. For simple PCBs, drilling may only need one file, but for complex PCBs there are number of files - for example where position of holes is on each layer and drill guide is usually just a PDF showing you where holes are placed on each layer, to visually check if the holes are correct.

2) a simple example of using a keepout layer can be marking the space under a connector which has some metal elements touching PCB - you may want to specify a keep our area, so a person who will be doing layout will not place tracks or vias there (the metal on component could possibly cause short circuit with tracks / vias on PCB)

Courtyard / Assembly layers: for some components, the space where they are touching PCB is not the same as they need to have around them, especially components with stand off or overhanging parts. So you need two layers - one which will show where to mount the component and another one which will show you the safe distance where you can place other components.

[qdrives]

1) I am unable to tell you the difference between the drill drawing and drill guide. All I know is that they are no longer used by fabricators so I would suggest to ignore them and hide them.

2) The keep out layer is used for various things to keep out of an area. There may be areas on your board where you cannot have components (SMD and TH pad) or other conductive elements. The keep-out layer applies to all layers. You can also place keep-outs on the individual copper layers which only applies to that layer.
In the past I used the keep-out layer to also prevent copper (polygons) to come to the board edge. Today we have the board clearance rule for that.


3) Via's and Through Hole pad are on multiple layers. That is why they are on the "multi-layer" layer.

4) These are the layers I have in footprints (library). Naturally, the colors are for your personal preference. 3D body, Component Center, Courtyard and Designator are "Altium standard" layer types. Polarity isn't.


5) I do not have an assembly drawing. Everything has a 3D body and that works better in my opinion.

6) I assume you mean courtyard when you mention "component boundary"?


This all results in the assembly documentation as attached here in the PDF.

[gyuunyuu1989]

Thanks, a response from the professional is always quite helpful.

You have declared several layers as layer pairs. These are 3D Body, Courtyard and Designator. Can't we just declare this as mechanical layers (not pairs) and then Altium is smart enough to work out the rest depending on whether we place a component on the top side of the board or bottom? I mean when we create PCB footprint, we place a 3D body, and a courtyard and a designator. Now do we really need to create a layer pair? If so, doesn't this mean that what shall have to manually place something on both layers i.e 3D body on both layer pairs, courtyard on both layer pairs e.t.c?

Also, what is the purpose of the single mechanical layer called Board? There is no board there since this is related to the foot print and not the PCB right?

[qdrives]

A "layer pair" is to tell Altium that it should 'flip' the contents when the component flipped layers.
Often, all things in the footprint will flip. I do not recall ever done something on 'single' layers in the footprint library.
Not having defined layers pairs in Altium can be a nightmare when you design boards with components on both sides and discover that you forgot to set up the layer pairs after many components have already been placed on the bottom. Better to set things correct in library.

Normal layers, as shown in the screenshot as "Board" do not flip. That layer is for the board outline. And you are correct, there is not board outline in a footprint library. I do not recall how it got there, nor why there is a internal plane 6. I should my script to see which component has something on these layers and clean things up.

[robertferanec]

1) when you start using uVIAs, blind VIAs, buried VIAs, through hole VIAs, drilling becomes complicated. For simple PCBs, drilling may only need one file, but for complex PCBs there are number of files - for example where position of holes is on each layer and drill guide is usually just a PDF showing you where holes are placed on each layer, to visually check if the holes are correct.

2) a simple example of using a keepout layer can be marking the space under a connector which has some metal elements touching PCB - you may want to specify a keep our area, so a person who will be doing layout will not place tracks or vias there (the metal on component could possibly cause short circuit with tracks / vias on PCB)

Courtyard / Assembly layers: for some components, the space where they are touching PCB is not the same as they need to have around them, especially components with stand off or overhanging parts. So you need two layers - one which will show where to mount the component and another one which will show you the safe distance where you can place other components.

[gyuunyuu1989]

A "layer pair" is to tell Altium that it should 'flip' the contents when the component flipped layers.
Often, all things in the footprint will flip. I do not recall ever done something on 'single' layers in the footprint library.
Not having defined layers pairs in Altium can be a nightmare when you design boards with components on both sides and discover that you forgot to set up the layer pairs after many components have already been placed on the bottom. Better to set things correct in library.

Normal layers, as shown in the screenshot as "Board" do not flip. That layer is for the board outline. And you are correct, there is not board outline in a footprint library. I do not recall how it got there, nor why there is a internal plane 6. I should my script to see which component has something on these layers and clean things up.

Isn't Altium smart enough to know that when a PCB footprint is flipped, everything goes upside down? Therefore, we don't use layer pairs for 3D body, Component Center, Courtyard, Designator, Overlay, Paste, Polarity, Solder. Rather, Altium is smart enough to know how things must be flipped depending on whether we are using SMD pads or through holes in the footprint.

[gyuunyuu1989]

I have used the Altium "IPC Compliant Footprint Wizard" and also the "Footprint Wizard". Neither of them create a footprint that has layer pairs for things like courtyard, 3D body, assembly e.t.c. I am confused now.