Matt's Altium Presentation 10/27/2022

Owned by Walter Stadolnik (Unlicensed)
Last updated: Oct 28, 2022 by Matthew McCauley
5 min read

Video Recording:

Panopto

About Altium Designer

  • Includes schematic + Layout in the same software - very nice, integrated solution, but kinda compl

  • Everything is parameterized - parameters are used for finding components, so consistency matters

General Altium Tips

General Shortcuts

  • Can press tab to pause whatever operation you’re doing if you need to tweak settings mid-action

Schematic/Symbol Tips

  • Space bar - rotate symbol

  • x/y - flip component over x/y

  • When you do CTRL+C, you can then click a point to be the “origin” of your selection - this is useful to make sure that your footprint stays in the right position with respect to the origin when you copy-paste it into your footprint

  • CTRL+W to route wires

Layout/Footprint Tips

  • Shift + S to hide all irrelevavent layers and focus on the active layer

  • CTRL + M to open the measure tool (CTRL + C to clear measurements)

  • Press 2/3 to switch between 2D and 3D view modes

  • press g to change grid size, R to flip metric/imperial

Creating a Project

  • Right click on license → Use

  • Make sure you’re signed into the NER vault

  • Right click on “Northeastern Electric Racing under Projects pane

    • Select “create project”

    • Use NER standard project

    • Enable Version Control on project so that you can revert if something bad happens

    • Automatically creates a schematic and layout file

Workflow

  1. Import/Create components

  2. Create Schematic

  3. Complete Layout

Component Creation

Symbol Creation

  1. Refer to this document for Component Creation requirements!

  2. Spec a component!

  3. See if there’s a link on Digikey/Mouser to an EDA download - Can be UltraLibrarian, SnapEDA, or anything else

    1. If you can’t locate any footprint or schematic symbol files, then you can use the footprint/land pattern info in the component data sheet as a guide to create your own files

  4. If using an EDA download, import the EDA files through ____. This will load a library into Altium (visible under the Projects tab) that contains the footprint and symbol

  5. Open explorer, and navigate to managed content → Symbols. Identify which category makes the most sense, and open that folder. Click “Add Symbol” to start a new symbol. Name it something relevant (i.e battery holder), and put something in the description relevant to the part. How generic you make the part name depends on how unique the part is/how easily it is to

  6. Create symbol by placing lines and pins, both of which are accessible from the toolbar at the top of the screen. When placing pins, make sure that the side of the pin with the small square on it is facing away from the part - this is the side that wires will connect to!

  7. Enter properties panel, and update the reference designator to the appropriate value (i.e. R?). Note that the “?” will be replaced with a part number when you place the component

  8. Once completed, save to server and put a relevant commit comment

Footprint Creation

  1. Same process to create the footprint as used for symbol

  2. Delete anything in the footprint that you obviously don’t need

  3. Copy-paste the footprint using CTRL+A and CTRL+C

  4. Open the View Configuration panel, and create the component layer pairs by right clicking on “Component Layer Pairs”, and filling in the name and layer number fields. Leave the layer type as N/A for all layer pairs. Refer to the table in the PCB Guidelines doc to make sure you get the layer numbers right

  5. Poke through each of the layers and see if anything is misplaced. If it is, move it onto the right layer by going into the Properties panel and changing the layer

  6. Add any missing details (things like component center are often missing)

  7. Make sure the 3D model is added to the assembly layer, and that it lines up properly with the footprint

About the Layers

  • Assembly - We use this layer to store the 3D model of the component being created.

  • Top Overlay - This is your silkscreen

  • Component outline - Should match the physical outline of the component package.

  • Courtyard - keepout region to make sure that you don’t have components too close to eachother. The PCB guidelines doc specifies how far this should be from the component outline.

  • Component Center - Used by pick and place machines to align components onto the board. Make sure this is perfectly centered!

Putting it all together

  • Open explorer, and navigate to Components

  • Create a new component in the folder relavent to the component type youre creating

  • Update the name, description, and parameters

  • Open Advanced settings → Make sure that the Folder is one that makes sense! For Type, click the category that makes the most sense for the part you’re creating

  • Click “Add footprint,” and select “existing footprint” to use the one you created

  • Click “Add Symbol,” and select “existing Symbol” to use the one you created

  • Save to server, and add some release notes. Put “Initial Release” if it’s the first release for the part.

Cloning Components

  • For common component packages (usually passives like resistors, caps, etc.), you should make the component by cloning a template part

  • For resistors, open explorer and navigate to the resistor folder under components. Right click on the resistor clone for the desired package (ie. 0603, 0804 etc.), and click -> operations-> clone

  • The cloned part should already have a footprint and symbol attached - all you need to do is update the parameters, description, and name, and you’re good to go.

Schematic Capture

  • Can access components through the Components Panel or the Explorer panel

  • Go to explorer, navigate to click and drag components onto the schematic page

  • Wire everything together using CRTL+W

  • To relabel all components reference designators automatically, use Tools-> Annotation->Schematic Annotation Configuration. You don’t need to tweak any of the settings for this from the default

  • left lick anywhere on the white space, and open the parameters panel to edit information about the document

  • Also right click ->options on the white space to enter information about the schematic sheet

Layout

  • Design → Import changes to pull in everything from the schematic to the PCB

  • Drag the room across the entire board area, then go to View options and hide the room. Rooms only really matter to organize large boards with repeating sections

  • NEVER hit x/y to flip a component in layout → this will [-------]. Instead, use L to flip a component from the top to the bottom layer

  • right click on a component → align → (selection) to align components and vias nicely on the board.

  • Typical PCB fab accuracy is down to the thousandths of an inch, so you can get pretty precise

  • Download the RUL file from the standards folder in drive and import it to make sure that the

  • When you think you’re done with the board, go to Tools → Design Rules Check in order to figure out what design rule violations exist. These error messages are typically very helpful, and they all need to be resolved before generating deliverables and manufacturing the PCB.