The Celtic Engineer is a weekly newsletter produced by Celtic Engineering Solutions. We hope you enjoy it. If you have any suggestions for topics, would like to give feedback or want your email added to the distribution list please send an email to [email protected].
How many layers are in your cake?
When I first started using Altium I found the mechanical layers very confusing. Once you know the secret you will laugh that anyone could be confused. The mechanical layers can be found by clicking on the current layer color bar in the lower left of the screen. This brings up the view configurations window. In the upper right of the window you will find the mechanical layer definitions. You can have up to 32 layers. The big secret is there is no agreed upon definition of what each layer should do. You can use them however you choose. I don’t know about you but knowing that was liberating. And then a bit daunting. What do I want to do with them? What do other people do with them?
That was where I started. I looked around to see what others were doing and how I might make use of them. In truth, I came up with two sets of them. Set 1 is what I want to talk about today. It is the set I use for making regular PCB’s that most everyone is familiar with. The other set, set 2, I use when I am making boards that have bare die on them. These boards are usually made of some kind of ceramic material as opposed to FR-4 material. They die do not have pins but pads where they are wire bonded. Needless to say, you need some pretty special equipment to build those boards. I will confine the discussion to boards that are more familiar.
Who’s on First?
While you can choose to use them however you want, I am going to make some suggestions that I think will be helpful. First things first, what to do with layer 1? This was an easy one. When you start a new project the most important thing you want to know is how big is the board. I place the board outline on layer 1. I don’t place anything else there so that it is easy to re-size the board if needed.
Layer 2 is often labeled board info. I use this to place directions to the person who is laying out the board (very often that is me). A good example of how I use this layer is for a JTAG box header. There is a notch that keys the plug and jack together. I like to place the notch facing away from the board because that is where the ribbon cable will be. It’s not a big deal, but I just put a note indicating which side to face away from the board.
Layers 8 and 9 are Assembly layers. Most boards have a silkscreen layer. If you are lucky, the board is huge and there is plenty of space on the board to place all the reference designators. I am rarely that lucky. I include a ‘.Designator’ string on layer 8 in the part library. When this special string is converted, it pulls the reference designator from the schematic and puts it on the Assembly layer. Since the Assembly layer is not on the board like the silkscreen layer is, you can do some neat stuff. For example, you can place the reference designator on the pads or in the middle of a big part. You wouldn’t do that with silkscreen because the ink would keep you from soldering to the pad and once the part was placed you would not be able to see the reference designator anymore. You are also limited to 50-70 mil height with silkscreen. Smaller than that and the ink tends to run together. I have made text 5 mils high and 1 mil thick. I know what you are thinking, no one can read that, unless you print it out blown up. This is a great advantage if there are many parts on the board and there is no room for the silkscreen. Your assembly drawing is a bit of a map.
You may have noticed that I said layers 8 and 9 are assembly layers. Top and bottom, of course. But it is more than just two layers. These two layer are tied together in what Altium calls a Layer Pair. When layers are paired, they will follow a part when it is moved from the top to the bottom of the board. Just like the reference designator on the silkscreen layer follows the part from the top to the bottom, the ‘.designator’ string on Layer 8 will get moved to Layer 9 when the part is moved to the bottom.
What are some other layer pairs? Layer 11/12 are for placing dimensions. Layer 13/14 are where 3D bodies are placed. Layers 15/16 are for the courtyard. You must explicitly pair two layers if you want them to be paired. This is done in the view configurations window. You will find a button in the lower left called Layer Pairs.
Your imagination can take you a long way. You can put a boarder around the PCB by placing this boarder on a layer. You can place tables and notes. If you get very adventurous and start placing parts on inner layers (yes it’s a thing) you will want a layer that you define as the cavity layer, I use layer 3.
If you glue your parts down you might have a glue layer, a stake layer or a glue and stake layer. The usages are really only limited by your imagination. My suggestion is to make a list and then make every board the same. Consistency is very important. Also, please talk to the people who will use the information you are placing on these layers and get some feedback from them. Since they are your customers (the consumers of your product) they should find the information useful.
In the View Configurations window, you may notice that not all 32 layer are displayed. There is a check box below the list that says ‘Only show enabled mechanical Layer.’ There are also 4 check boxes for each layer. Enable allows the use of the layer. Show will display the layer. Single is used for single layer mode and Linked To is for linking to a sheet where you make your own templates.
This newsletter is sponsored by Celtic Engineering Solutions LLC, a design engineering firm based out of West Jordan, Utah, which can be found on the web at: www.celticengineeringsolutions.com. You can find the newsletter on the company blog, LinkedIn or by subscribing. Send your emails to The Celtic Engineer at: [email protected].