Altium Layout Cheatsheet

Project Workflow and Shortcuts for Altium Designer 2020 - Schematic Tool

Creating the board

ProjectName.PrjPcb » Right Click » Add New to Project » PCB
PCB1.PcbDoc » Right Click » Rename(as desired)

Configuring the Board

Set the Origin

Edit » Origin » Set

Set Units

View » Toggle Units (Hotkey: Q)

Set Snapgrid

Hotkey: G
Hotkey: Ctrl+Shift+G
(Opens snapgrid settings rather than swap between predefined snapgrids)

Edit the Board Shape

Ctrl+PgDown: Zoom Fit
View » Board Planning Mode (Hotkey: 1)
Design » Edit Board Shape
Adjust Board corners until desired board shape is achieved

You can also redraw with
Design » Redefine Board Shape
Draw the polygon fill to create board

Transfer the Design

from schematic

Design » Update PCB Document Name.PcbDoc

from PCB

Design » Import Changes from Name.PrjPcb
Validate Changes
Execute Changes

If you’re missing any footprints you’ll get an error when you try to import

Setup Layer View

Panels » View Configuration (Hotkey: L)

Setting Up the Stackup

Design » Layer Stack Manager (Make sure to save!)
Panels » Properties
Properties » Enable Stack Symmetry

Set up Planes and Signal layers (Standard is 1 oz. copper. If it’s a high power board 2 oz. may be necessary but for hobby projects realize 2 oz. is expensive!)

Via Types » Ensure through hole via is present(If you need partial/embedded vias you’ll be able to figure it out here on your own)

Remember to save the stackup!

Before you Place Set Up Your Snap Grid!

Basic Electrical Rule Configuration

Here are some basics to get you started, ICs tend to have metric based packages so probably best to use mm here.

Route Width: 0.25 mm Where: Routing Grid Design Rule (Can also do whatever 50 ohm impedance is for your dielectric/stackup)
Clearance: 0.25 mm Where: Electrical Clearance Design Rule (High speed signals need special care!)
Board Definition Grid: 5 mm Where: Cartesian Grid Editor
Component Placement Grid: 1 mm Where: Cartesian Grid Editor
Routing Grid: 1 mm Where: Cartesian Grid editor
Via size: 1 mm Where: Routing Via style design rule (High current traces may need larger/multiple vias)
Via hole: 0.6 mm Where: Routing Via Style Design Rule

Altium Support Polar Grids if you’re doing a curved board but I’m not going into that

Cartesian Grid Editor (Hotkey:Ctrl+G) Set the grid definition here as well so you can see it well

PCB Rules

Design » Rules
Set up everything according to what your manufacturer supports. Some manufacturers will provide an Altium rule file to import, and if they do love them eternally because so much less busy work

Basic setup

clearance: 0.25mm for all
signal: 0.25mm standard
power: thick traces, minimum can still be low for small offshoots to pins, etc
routing vias: 1mm diameter, 0.6mm hole size

Yes, you can be more specific, and if the board’s high density please look in depth at your manufacturer’s capabilities. If it’s a hobby project, who cares :)

Placement

My first boss taught me that 90% of the battle is placement, and I recommend you take his advice.

Spend time making the rat’s nest of traces as short as possible. Rotate parts around, and make sure there is as short of a distance as possible for you to route wires.
Place Connectors and any mechanical requirements First, then place components as fits.
Make sure you place the bypass caps as close as physically possible to the VCC and GND pins of your components!
If you need to use vias use them, there are different theories on what’s best here. Some people prefer routing all on the top layer, some believe hiding the signals in your stack up is more beneficial.

I’ll point you to Henry Ott (hottconsultants.com) if you want to read up on the different stack ups and routing techniques I also hear good things about Howard Johnson, and John Howie(totally different names, not clones or anything) has some stuff on EMC, but it’s a bit harder to find

Planes

Place your planes now!

You need to have a small keepout area on the edge of the board to make manufacturers happy

Polygon Pour » Draw » Click Polygon » Properties » Assign Net » Repour
(If you mess with things be sure to repour, it’ll fix some weird issues)

If you think yourself a genius feel free to attempt to split your ground planes, if you’re like the rest of us mortals do the best to ensure your board has as solid of a ground plane as possible.

A solid plane rather than a split one is almost always better.

Basic Routing

Route Mode (Hotkey: Ctrl+W)

Connect everything with the shortest trace possible! Highest priority signals get routed first, remember some lines need controlled impedance/differential pair routing
Route slow speed traces last
Make sure to put vias to prevent any dead copper!
There are fancy methods of making high speed transmission lines with vias along fancy traces but that’s application specific
In general spread some via stitch out around the board after to help with return paths. The person who taught me taught me to do it pseudo randomly to prevent “resonance of something”. I can’t quite remember everything ¯_(ツ)_/¯ , but he’s a pretty bright guy so I’d assume he was right.

Autorouting is a privilege you earn after you learn when to use it. If you’re starting out you don’t know how to and shouldn’t. It can save time in some cases but I avoid it 95% of the time

Boards Done -> Design Rule Check

Tools » Design Rule Check

Fix or approve any errors

Check your board out!

Press 3 to view the board in 3D, make sure everything looks alright
Press 2 to go back to routing mode

Fabrication Outputs(Getting your board made!)

You can either output individual files from

File » Fabrication Output
File » Assembly Output

You can also export to other tools such as HyperLynx (super fancy sim software for EMI that you’ll only get to play with if your company has a license) from the file tab.

You can print PDFs from here as well, Altium can output 3D pdf files that allow rotation and zoom in Adobe Acrobat almost as if you were looking at the assembly in Solidworks.

Setting Up Output Job Files

This will output everything you want, think of it like the CMake of Altium

Right Click Project » Add New to Project » Output Job File

Save file with desired name

Basic set of outputs to set up in the .OutJob file

Fabrication » Gerber » PCB Document
Fabrication » NC Drill Files » PCB Document
Assembly » Generate pick and place files » PCB Document
Documentation Output » Schematic Prints » (single page for basic setup)
Documentation Output » PCB Prints » PCB Document

Configuring the outputs

To Configure each output right click and hit configure
Gerber Config - (Format, 4:4, Units:mm, layers » plot layers » used on, advanced » position on file » reference to relative origin)

Set up the output container

Click the folder structure in output containers.

Now check the enable box for every file you want in that folder.
Set the top file path to manually managed.

I recommend you store everything in a folder called outputs because it looks better.

You may want to go into advanced and enable auto load of gerber and NC drill outputs so you can check to see if they’re accurate after being created

Click the PDF Container and add your PDFs to it, adjust this output structure as well. Name it as you’d like and configure auto open if you want

ODB++ is a new format that contains pick and place info alongside board info. Fancy board houses like it. If you’re getting high quality boards or a large number of boards made please just communicate with your board house/assembly house. They’ll tell you what they prefer, and if you give them what they prefer it’ll save you a bit of money hopefully

We’re going to add our BOM to the output as well, but we need to set it up first

Active BOM

Right Click Project Name » Add new to project » Active Bom
Properties » Set Production Quantity to see best prices

Now go through each type of component and select the manufacturer you want to buy from, Once you select the manufacturer give it a user rank by making a star rating.

Once you do this the status message on the far right side of the BOM should become a green check box for the items that were in stock.
Add vendors’ links for any products that still need them by clicking the part and doing add solution.

If you replace a part with a new solution note that whatever option has the most stars will be used if available.
(ie: if you have 2 different types of amps you can use but the preferred one is usually out of stock set the preferred to 5 stars and option 2 to 4)

If you entered the production amount the tool will help you pick from the different distributors and ensure stocks.

Save the bom and the project!

Now go back to your output job file and add the bom, I recommend you customize it and add either the single supplier or double supplier template.

Add it to your output folder container!

Wrap Up

Save everything! You can reuse things like rules setups and your output job file for most cases!

Now go into your output job file and click your output containers. Click generate content for each and ensure it’s correct.

Now you have the pdfs of your schematic and board to share with everyone and your manufacturing files! You’re all set to have it made