Congrats on finishing the schematic! At this point you should have no validation messages and have had a lead look over your schematic.
Settings
A copy of the settings I use can be found here: Altium Settings
Importing these should make it a bit easier to follow along, and it configures some of the defaults we use such as text size, etc.
You can import the full settings by clicking the settings icon in the top right next to the workspace name, choosing load from file in the bottom, and selecting the DXPPrf file. If you have already been using Altium and have custom settings you want to keep, you can just import the PCB defaults in PCB Editor → Defaults, and loading the dft file.
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 Design → Layer Stack Manager and then 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.
Component Placement
Moving Components
To move a component, you can click and hold them while dragging your mouse. Where you initially click on the component will determine where the snap point will be. For example, if you click and drag from the centre of a part, it’s the component origin that will snap to the grid. However, you can also click and drag from a component pad / hole, and it will be that feature that snaps to the grid instead. The snap point is shown by a green cross extending across the screen while you’re dragging.
You should almost always be dragging components by their origin, usually located in the middle of the part. Otherwise, components will no be aligned to the grid.
General Guidelines
Below are some general placement guidelines. There are of course a bunch more, and we will mostly gloss over the “why” here but I do encourage you to ask a lead about them when you get the chance!
Rat's Nest
You may notice that there are a mess of lines between the component pads. These represent the connections that need to be made between pads according to your schematic. It might be messy at first, but use these to help you place components in such a way to minimize the number of connections that need to cross over each other!
Resistive Dividers
Resistive dividers should be placed close to the device which needs it, keeping the length of the “divided” net to a minimum. In the example schematic, the VBAT divider formed by R1 and R3 should be placed close to the op-amp U1 rather than the input connector.
Decoupling Capacitors
A decoupling capacitor is a device that supplies charge to an IC. These should be placed closed to the ground and power pins of the device as to minimize the “current loop”. Recall that current flows always in a closed loop. To visualize the size of the current loop, you can draw the path the current takes from the positive pin of the cap to the positive pin of the IC, through the chip to the gnd pin on the IC, and then to the gnd pin of the cap.
In this example, the current loop on the left is smaller than the one on the right! Realistically both of these are not too bad, at least the cap is next to the component.
Connectors
When placing connectors, keep in mind that they are quite tall relative to other components, and are keyed on one side. This means there is a locking ramp that you have to push on to unlatch the connector, you can see this in the 3D view by pressing “3”. Make sure to leave space for your fingers!
For this reason, generally connectors are on the edge of a board with the lock facing outward. You should especially avoid placing connectors such that the lock is facing each other and very close together. It will be hard to get your finger between those connectors to unlatch them.
Board Shape
Now that you have completed placement, you can adjust the shape of the board to fit your components.
In the bottom of the screen, you’ll see a bunch of tabs for all of the drawing layers in the design. Click on the Keep-Out Layer, and here you can draw the shape of your board using lines and arcs. Board dimensions should be in full mm, so set your grid accordingly!
Once you have a closed outline, press Shift + K to isolate only elements on the Keep-Out Layer. Window over all elements to select them, and convert that to your board shape using Design → Board Shape → Define Board Shape from Selected Objects.
Routing
Ideally during the placement process, you’ve started to form an idea of how you’d route things and placed your components in such a way to make this process as easy as possible!
Traces
To draw a trace, press Ctrl + W. If you move your mouse to the centre of a pad, you’ll see it snap in place when there is a green cross and a circle. Drag your mouse to draw out the trace, click anywhere to create a vertex, and click again or click on the centre of a pad to end the trace.
Some general rules of thumb:
0.25mm trace thickness unless you require otherwise
Avoid acute angles
Route all traces except for ground, we will make those connections later!
Vias
Sometimes you may find that traces need to cross over each other. If this is the case, you can connect traces on different layers using a hole plated with copper, called a via.
We have a 2 layer board, which means signals can cross past each other on opposite layers. In my routing, I have used a via to allow the 12V trace to cross below some other components on the bottom layer (blue).
Polygon Pours
Now that all connections except ground have been made, we will connect all the grounds together by filling all remaining empty space on the board with a ground plane.
Use the Place Polygon Plane option in the top bar, and define the 4 corners of your polygon. Note that you don’t need to make the polygon definition the same shape as your board. You can use a rectangular polygon to cover a board with rounded corners, the copper won’t be poured where there is no board.
Cover both the top and bottom layers with a polygon, and assign the net to gnd in the properties panel, You should see that all ground pads are now connecting to the place through small tabs.
It’s also good practice to place a gnd via next to every gnd pad. While they might all be connected through the top side copper, the pour has to snake it’s way around all the traces and components. Having gnd vias ensures a direct connection through the bottom layer.
Silkscreen
The silkscreen comprises everything that will be printed on the exterior of the boards for labelling, etc. These are the Top and Bottom Overlay layers. If you click on the top overlay layer, you can more easily select and rearrange the component designators.
While on this layer, you can also add labels for the connectors as well as the board name and Midsun logo.
To add the logo, you can use Place → Graphics and draw out the area where you want the image to go, then selecting the file.
Design Rule Checks
For major rule violations, often the program will alert you in the form of green circles with crosses. However, this is not always the case. Near the end of your design, go to Tools → Design Rule Check → Run Design Rule Check, and address any issues in the report. Note that you can click on the hyperlinks to cross-probe to the affected area!
If you have no warnings or violations, get a lead to look over your board, you might be done!
