Altium
Altium Designer is the preferred PCB design tool for use in the group. It provides a modern interface, access to some professionally designed part libraries, and good support for RF routing when compared to free tools, so it's worth learning!
Access
In order to install Altium, you must first contact Joel in order to sign the end user agreement. Once that's in place, contact David Moore in order to use his Altium account to download and install Altium on your computer.
During installation, you must log in with the Altium account, and then specify the license as coming from a private license server using the following info:
sever name: license-altium.engin.uimch.edu <br/> server port: 22921
After this your installation should work without issue. If you get license problems, double check that it is getting the valid license from the server.
Tutorials
Altium provides very good documentation and tutorials, which can either be accessed through their website or pulled up in Altium itself. Selecting Help -> Getting Started with Altium Designer provides a page with links to several useful pages. Specifically, Getting Started with PCB Design walks you through most of what you need to know.
Finding and Downloading Premade Part Libraries
Altium has a fairly large assortment of downloadable part libraries which provide schematics and footprints for various components. When selecting parts to design your board with, it's a good idea to check whether it has a premade footprint, because it can save you a good deal of effort.
New Way: The Vault
You can easily access every part in Altium's libraries by connecting to their "Design Content Vault". Use these steps to add it:
- In the top menu bar, go to
DXP -> Preferences - Select
Data Management -> Vaults - Press the button labeled "Add Altium content Vault".
- Press "Apply".
To browse the Vault, either choose DXP -> Vault Explorer or use the buttons in the bottom right of Altium to go to System -> Vaults. The Vault can also give you up to date part prices and quantity in stock from suppliers like Digikey and Mouser!
Old Way
To access these libraries, you simply need to visit https://designcontent.live.altium.com/ and login using a valid Altium account. Searching for part numbers is effective in finding ICs and discrete devices, and searching for connector names and putting in a bit of effort can usually yield appropriate footprints for things like SMAs.
After downloading the library you can simply extract in and place the resulting .IntLib file in the default public library directory, in order to keep things organized. By default, this is located at:
C:\Users\Public\Documents\Altium\AD14\Library
To use the libraries, open up a schematic and go to Design -> Add/Remove Library. It's best to add the libraries under the Installed tab. After adding them here, they'll be available in the when you search for components to add in the schematic editor.
Version Control
Altium has built in support for subversion in a way that is so easy to use that there's no excuse not to. This makes it easy to revert to earlier versions of your board, or to compare what has changed between an old board design and a new one. It can be enabled in DXP -> Preferences. More info will be added here at a later date. Ask David Moore if you would like more details.
Tools for RF/Analog Layout
For many of our PCB designs, the layout requirements can be a little more complicated than in low frequency digital boards. Fortunately there are some pretty easy steps you can follow to get good RF layout.
Microstrip Ground Plane Spacing
For nets carrying an RF signal, you generally want your trace to be 50Ω microstrip. On a typical 4-layer board, with a ground plane on the second layer, a 16mil trace width gives you 50Ω. However, this assumes you don't have ground plane on the top layer of the board, which you should. In order to keep the impedance correct, you simply need to tell Altium to pull back the ground plane from your RF traces.
The first step is to let Altium know which traces are RF traces in the schematic. In the schematic, first right click and choose Place -> Directives -> Net Class as shown below.
Move the created label so that it is attached to your RF net. Then double click it to bring up the parameters window, and edit the parameters so that they appear as shown below.
Now Altium knows that this net (and any other nets you attach this net class to) is an RF net. At this point we just need to tell it what to do with that information. We do this by setting up PCB Rules.
After opening your PCB, select Design -> Rules from the menu. This opens a window containing all the rules which Altium forces your layout to adhere to. All of these can be useful in getting your layout to do what you want to do. In our case, we will create a new Clearance rule.
Expand the electrical category and right click "Clearance", the select "New Rule...". This will add a new rule, which we can then edit. Change the rule name to RF_Clearance, and then type in the "Full Query" boxes as shown below to specify that you want a clearance between Polygons an nets belonging to the RFNets class that we created earlier. Finally, specify the clearance to be (at least) 20 mils.
Now when you go to pour your polygons, they'll stay far away enough from your RF Nets to keep your impedance correct!
Vias
Having good ground and power plane connections is important to boards working at high frequency, so you should pay attention to your vias. There are two things to look at specifically. First, you want to make sure that thermal reliefs (eg. spokes) are only being inserted where you really need them for soldering, and not on vias which are intended to give low inductance ground connections. Second, you want to make sure your entire ground plane is stiched together to the top ground pour with many vias, so that it doesn't cause any weird resonant structures. This can be done by hand or using the via stitch tool.
Thermal Reliefs
To get the right behavior for thermal reliefs, you need to edit your "Plane" rules. To keep it brief, it's easiest just to look at and copy the configuration shown below for the "Plane Connect Style" and "Polygon Connect Style" rules. To learn how to edit PCB rules, read the "Microstrip Ground Plane Spacing" section above. Note that you should edit the priorities of the rules using the "Priorities" button in order to ensure that the more specific rules take precedence over the more general ones.
File:PolygonConnectViaRule.png
Stitching
To insert ground vias by hand, simply choose Place -> Via or click the "Place Via" button. Before placing the Via, hit the "Tab" key in order to bring up the properties, then change the net to GND. You can also edit the size. You can then place this via, and copy it all over the design, letting Altium make the correct plane connections.
To use the via stitch tool, select Tools -> Via Stitching/Shielding -> Add Stitching to Net. You can edit the parameters here, and then Altium will try to insert vias on the net you selected. Play around with settings to see what gives you good results.
Split Power Plane
Sometimes, having separate internal power planes on the same layer can be helpful/necessary. Fortunately, this is pretty easy to configure. When you set a layer as a "plane" layer in Altium, you can draw on it in the negative, effectively drawing cuts. Simply use select the appropriate plane layer at the bottom of the layout window, the use Place -> Line in order to draw cuts. Once you have isolated the two (or more) regions, right click and select "Properties" in order to choose which net to connect each region to.
Importing Complex Microstrip Layout
If you want to use more complicated microstrip techniques (such as microstrip filters), it may be beyond what you can easily do in Altium. Agilent ADS is the best tool for designing these sorts of things, but how can you integrate that with your PCB? It's not seamless, but there is a way to import externally drawn layout into Altium. Also, unlike many free design tools, Altium can detect when nets are connected in the layout by shapes, and won't pester you about them being unconnected.
To see how to import RF layout, check out this video: How to Import Graphics and RF Geometries Using DXF Files