Congrats on finishing the schematic! At this point you should have no validation messages and have had a lead look over your schematic.
Importing to Layout
Go to Design → Update PCB to port over your schematic design to the layout. After hitting execute changes, you should be brought to the PCB design tab.
Configuration
Origin
The origin is represented by a white X overlapping a circle. By default it’s some distance off to the bottom left corner of the board. We will move this to the bottom left corner to allow us to more easily place parts in specific areas of the board, such as exact centre, etc.
Since the default unit is imperial, if we want the origin to snap to the exact corner we need to use an imperial grid. Press G and set the grid to 100mils, and use Edit → Origin → Set and click the exact bottom left corner of the board.
Grid
In contrast to the schematic, the PCB should use all metric units. Now that the origin is set in it’s new final spot, we’re free to change to metric. You can switch in the properties panel, or by pressing “q” and observing the units in the bottom left corner of the screen.
The grid configuration is much more dynamic, as it dictates the physical placement of components on the board. For any situation, I like to use the largest practical grid to help keep things aligned. Just like the schematic, you can change the grid by pressing “g”. Note that 1 mil is 0.001”, and not 1mm. Please stick with metric! Here’s a short list of common grid values I use, I always start with the largest unless I have a reason to go smaller:
Connectors and ICs: 1mm or 0.5mm
Passives (resistors, capacitors, etc): 0.5mm, 0.25mm/0.1mm if needed
Routing: 0.25mm, and rely on the snap feature to align traces to pins
If you use too small of a grid, its a lot harder to make sure everything is aligned and evenly spaced. I’ll be sad if you have a row of resistors that are 0.01mm out of line with each other!
Stackup
A PCB is composed of many layers of copper and insulators (dielectrics) sandwiched together into a panel. The stackup is wat defines the details of this construction, such as the thickness of each layer and it’s material properties.
We will be using a 2 layer board, meaning there are 2 conductive copper layers where we can route electrical signals. You can load a preset for the stackup we use by going to File → Load Stackup from Server and navigate to Managed Content → Templates → Layer Stacks and select JLC 2L 1oz 1.6mm. 1.6mm refers to the approximate thickness of the finished board, and 1oz refers to the thickness of the copper layers. Why thickness is measured in ounces is beyond me (these Americans amirite), but 1oz copper represents the thickness of 1oz worth of copper spread evenly over 1 square foot. That equates to about 35um.
Design Rules
Design rules dictate the complete set of physical design constraints to ensure that the board is manufacturable. For example, this is where you would define the minimum trace width and spacing, component clearances, etc. JLC’s capabilities improve every so often and are listed on their site, however you can grab this template (maintained for now by f39zhou) and load it through Design → Rules, right click Design Rules in the tree on the left and click Import, click ctrl + A to select all, and then load the 2L 1oz rule file. Hit Yes to the prompt about clearing existing rules prior to import.
Board Shape
Altium will generate a default board shape, which is shown by the black rectangle. The components from your schematic should be off to the side.
Before you’ve started placement, its hard to determine how large your board should be, so typically I’ll leave the default size until I have a better sense of what the dimensions will be.