Tutorial

Learn the basics of circuit design and PCB layout.

Go to the ece download page to accept the licensing agreement and get instructions on obtaining the software and accessing the server.

Make sure you have a VPN connection to the ECE network.
Start Altium and from your "My Account" page:
Click on "Setup private license server"
Server name: xxxxx
Server port: xxxxx
Select the new license that appear and click on "Use"
You may as well also delete any old, expired licenses that are also showing.

By default, all components are numbered with a "?" (eg. R?). You must number these before simulation or layout because all components need a unique identifier. First, you may (optionally) remove all existing numbers. This is useful if you think you might have some duplicate component numbers:
Tools / Reset Schematic Designators ...

To have Altium automatically number all un-numbered components:
Tools / Annotate Schematics Quietly ...

Double click on each missing component
Click "Choose" in the "Library Link" window.
Select the part from the current library.

Or select Tools / Update From Libraries ...
You can change the source library for all parts from here.

Hold down Ctrl while dragging or select the object and click
Edit / Move / Drag

To change the default behaviour from moving to dragging:
Tools / Schematic Preferences / Graphical Editing / Always Drag (check box)

For more information visit the following link.

Yes. Double-click the component on your schematic and select the layout you want from the drop-down box next to the footprint name. If there is no drop-down box, you do not have any other options and you will have to replace the entire component. After making this change, update your PCB (Design / Update PCB) and you will have a new footprint.

Alternatively, you can change the footprint on your PCB layout by double-clicking the component and choosing a new footprint in the associatted drop-down box. You will get a lot more options doing it this way but you will lose the change next time you update your PCB from your schematic.

Edit the simulation parameters (step 2) to set the initial condition and ensure that the "Use Initial Condition" box is checked in the simulation configuration window (step 3).
Analysis Setup (wrench) / Transient Analysis / Use Initial Conditions.

Warning: On an unpolarized capacitor, it is ambiguous which terminal is which. If you set an IC of 5V and notice that you get an IC of -5V in your simulation results, rotate your capacitor by 180 degrees and try again.

You can change the "Transient Stop Time" in the simulation configuration screen. De-select the "Use Transient Defaults" box to get access to the "Transient Stop Time".
Analysis Setup (wrench) / Transient Analysis configuration screen.

Warning: If you make the simulation time too long, it can take a very long time to execute which may tie up your computer and make it freeze. If this happens, see below.

You have 2 options:
1) Add a PCB to your project
2) Run the PCB Wizard (Files tab / New from template) and move the resulting PCB to your project

If you add a blank PCB, the default rules will be applied and you will have to check and change them by clicking Design / Rules. Routing Width and Electrical Clearance correspond to minimum tracksize and clearance respectively.

If you run the wizard, you will be asked about the design rules. The following are a good set of standard choices:

Metric
Custom board
50mm x 50mm (uncheck the Title Block, Legend and Dimension Lines boxes)
2 Signal Layers, 0 Power Planes
Thruhole Vias Only
Through-hole components / One Track
Minimum Track Size = 0.2mm (8 Mil)
Minimum Clearance = 0.2mm (8 Mil)

Note: It is very important to define the Minimum track size and clearance values properly or the Auto-Routing function will not work properly since Auto-Routing will not lay down any traces that violate these rules. You will be forced to manually route your PCB.

From your schematic, update the PCB (Design / Update ...)
Validate all changes on the ECO and execute them.

On the PCB, arrange all your components where you want them.
Auto-route the traces (Auto Route ... / All)
Manually change the traces to optimize your board if desired and add in any traces that auto-routing was not able to place.

It's ok to go ahead and design your PCB on the default 6x4 inch board or any board size that gives you enough room for all of your components. Once you are done, you can re-define the board shape and size.

Select layer "Mechanical 1".
Erase any existing lines and click (Place / Line) to draw a box. This tool clips the corner of your box that that is a nice feature on most boards.
Select all lines (Edit / Select / All on Layer)
Select (Design / Board Shape / Define from selected objects).

Adjust your "Keep Out" layer to be a little smaller than the board so that you can use it up without any traces landing too close to the board edge.

When you export your board to Gerber files, use the "Mechanical 1" layer as your "Cutting Outside" file. The PCB mill will route this shape out for you..

Refer to the following flowchart for the complete design path of a PCB.

You need the following 4 files: xxx.gtl, xxx.gbl, xxx.gm1, xxx.txt
You can generate them by selecting:

File / Fabrication Outputs / Gerber Files
General: Inches, 2:4
Layers: GTL (Gerber Top Layer), GBL (Gerber Bottom Layer), GM1 (Gerber Mechanical 1 - contains your board outline)
Apertures: Embed apertures (RS274X) should be selected
Results in: CAMtastic1.cam, xxx.gtl, xxx.gbl, xxx.gm1

File / Fabrication Outputs / NC Drill Files
Inches, 2:3
Select "Generage separate NC Drill files for plated & non-plated holes"
De-select "Generate Board Edge Rout Paths"
Results in CAMtastic2.cam
From CAMtastic2.cam:
File / Export / Gerber ...
Results in: xxx.txt

Select (Design / Board Layers & Colors)
Select (All Layers Off)
Select "Show" box for: Top Layer, Bottom Layer, Mechanical 1, Keep-Out Layer, Top Overlay, and all System Colors
Select "Apply" and then "OK"