Welcome to Laser Pointer Forums - discuss green laser pointers, blue laser pointers, and all types of lasers



Altium Designer - A quick start guide

Things

New member
Joined
May 1, 2007
Messages
7,535
Points
0
OK, so I've had quite a few people PM me asking hao2Altium, and while all the information you could ever need to get started is available on the internet, it tends to be scattered all over the place.

So, what I'm hoping to achieve with this is a basic "kick start" into Altium and the basics on how to use it. Note that Altium is an _extremely_ capable program, and what I'll touch on in this guide is basically just scraping the surface on getting a PCB together.

However, having said this, it is good to have a bit of understanding about PCB design first, such as trace width and via current handling capacity, your component footprint types, and also manufacturing parameters such as clearance and size constraints.

I will be splitting this guide up, just to make it a bit less tedious to read all at once, and so I can give my fingers a break :D

[size=+2]Getting Started with a new Project[/size]

The first thing you'll notice when you have installed and opened Altium is this panel on the left, called the Files or Project panel. This is the main form of navigation in Altium, so keep it around.



You'll notice quite a few options in this panel, but 99% of the time, you'll be using the PCB Project option. However, you could also use the Schematic option if you just wanted to create a schematic, and weren't planning on having it fabricated.

So, go ahead and start a new PCB project. You'll notice the Project panel is now showing your new project, with no documents added.

Altium works a little differently to most PCB softwares I've used, in that everything is separate. All your PCB footprints and schematic symbols are stored in separate "libraries".

Right click on your project in the list, and go to Add New to Project -> PCB Library, then repeat and add a Schematic Library, and finally, a Schematic. Don't add a PCB just yet.

You'll now have your libraries and schematic document under your project. If you notice they appear under a "Free Documents" tab instead, simply drag them back into your project.



At this point, go ahead and save your project. It'll ask you to save all your project files separately, so create a new folder for each of your projects to keep them organised, as you'll end up with a lot of files along the way.

Now, open your schematic sheet, and there's your canvas!

Across the top you'll notice a bar with lots of icons on it, which I guess you could call the toolbar. In particular, the ones towards the right side.



By hovering your mouse over them, you can see what they're for, so I won't explain that.

To the top right you'll notice a few little symbols, like the ground symbol and a resistor symbol. These are shortcuts to adding common components, and is easier than finding them in the libraries each time.

Click on "Add Part", and in the pop up window, hit "Choose". The top dropdown box should contain a few stock libraries, such as Misc Devices and Misc Connectors. However, while browsing through these, you'll notice there's actually very few inbuilt footprints and parts. Even if there is a part in there you need, it may not have the right footprint either!

Just for now, choose a part and hit OK, then OK again on the popup window. You can now drag your part around the schematic! Now, before you place it, there are a few handy shortcuts you should know. You can rotate the component using space, flip it in X and Y using X and Y keys respectively, and you can also hit Tab to bring up the component properties. Click to place the part.

Controls are pretty much universal through Altium, CTRL + Scroll wheel for zoom, scroll wheel by itself for Y movement, and Shift + scroll wheel for side to side. You can change these in the preferences if desired.
 
Last edited:
  • Like
Reactions: ARG



Things

New member
Joined
May 1, 2007
Messages
7,535
Points
0
[size=+2]Creating custom component footprints[/size]

So, unless your project is switching an LED on and off with a transistor, you'll most likely have to create your own component footprints at some point. This is where the PCB and Schematic Libraries come in.

The PCB Library is the place all your physical component footprints are stored, while the Schematic Library is where the pin definitions and schematic symbols are stored, and linked to your PCB footprints.

Doubleclick on the PCB Library to open it up, and along the bottom of the Projects tab, you'll see multiple tabs, one right at the end called "PCB Library". Click on it and you'll now have a list of component footprints you have created, which of course at this stage will be none, so a blank component. Now, at this point, figure out what component you're going to draw.

Conveniently, Altium has a built in component footprint wizard, which you will be able to use for at least 95% of your components, how handy is that? You can access it by going to Tools -> Component Wizard.

This wizard will walk you through step by step, asking details about your component (Which can always be found in the datasheet), easy done!

However, there will come a time when the component you need doesn't have a standard footprint, such as connectors. For these, you will have to create them manually, but not to worry, it's easy to pick up!

First, read the layout in the datasheet, and understand how all the pins of your component are laid out, and see if you can find a common dimension. For example, if all the pins are spaced 1.27mm apart, then you can set your grid to 1.27mm and just place pads or holes on the snap grid!

To set the snap grid, go to View -> Grids -> Set Global Snap Grid, make sure you specify the units. Across the top once again you'll notice your toolbar, select the "Place Pad" button. Straight away you'll have a pad attached to your cursor and ready to place - but wait, you haven't set any dimensions for it! Hit tab, and you'll get the pad properties window.



From here, you can set the pad hole size, it's shape, designator and other various properties. If you are trying to make a SMD pad, click on the Layer dropdown and scroll up, and select Top Layer. Don't worry if this component will eventually end up on the bottom of the board, Altium will take care of it. You can usually leave the Testpoint settings, solder and solder paste expansion properties alone. Once you have configured your pad, hit OK and go ahead and place it! Up the top left of the workspace, you will notice 4 sets of coordinates, X, Y and dx/dy.

Every time you place a pad, the dx and dy coordinates will zero to that location, so you can place your next pad relative to the last. If you have a large number of pins to place, there is an easier way.

Simply select your first pad, and copy it. Your cursor will change to a crosshair, and this is to set the copy reference point. Just set it to the center of the pad. Once you click the reference location, the pad is now copied. Go to Edit -> paste special, and select Paste Array. You can now specify the number of pads you wish to place, their X and Y spacing, and also how the designator increments. Most of the time the designator will increment by 1, however there is times when you may want it to increment by a certain number. Click OK, and you will now have the crosshair cursor again, waiting for you to select where the first pad should be placed. Click next to your previous pad and bingo, lots of perfectly spaced pads!

Next, you'll probably want to add some sort of silkscreen outline for your component. Click the "Place line" button, and then press Tab again. Here you can specify your line width, and also which layer it is on. For silkscreen, you will want to select Top Overlay from the dropdown. You will know it is on the correct layer as the line will appear yellow, if it is any other colour, re-check the layer it is on (You can change previously placed objects by rightclicking and going to Properties).

Make sure your new component has a name in the left tab (Doubleclick to change it), then save!

 

Things

New member
Joined
May 1, 2007
Messages
7,535
Points
0
[size=+2]Schematic symbol and pin definitions[/size]

Yay! You now have a footprint for your component! But you can't simply add this in your schematic, as it has no schematic symbol or pin definitions!

In the projects tab, along the bottom where you clicked PCB Library previously, click back to Projects.

Next, doubeclick on Schematic Library to open it up, and click SCH Library along the bottom tabs again. This window is a little different to the PCB Library, however once again you'll notice a list of components on the left. Doubleclick on Component 1, and it'll bring up a properties window. The first option you'll want to set is the component designator, which is what it'll show up on your schematic as.

So, if you're creating an IC, you'll likely make the component designator U? . By placing a ? at the end, it means the part will be automatically assigned a designator later on. You can also set a comment for the component, such as it's part number or type. To change it's name in your libraries, change the Library Link - Symbol Reference field.

Next, you need to tell it to use your footprint you just created! So in the Models field bottom right, select Add, and Footprint. Click Browse, and find your PcbLib in the dropdown menu. If it doesn't appear, you probably didn't save your PCB library! Your part will show up in the list on the left, so select it. Done! Your footprint should now show up in Models.

Next, you'll need to create the symbol that your component will appear as on your schematic. Note that if you are making a common component, such as a resistor or capacitor, you can use the built in schematic symbols and simply change the footprint - I'll cover that later.

Now, click into the workspace area with the grid, and press "p", and "p" again, this is a shortcut for "Place Pin". Now press Tab, and you can edit the properties of your pin. The designator of the pin needs to be set to the same designator as the physical pin on your component footprint! You can change the display name to something easy for you to remember, such as Vcc, GND etc, it is simply a visual reference as to the pins function and doesn't determine what it'll connect to. You can also edit the graphics properties of the pin on the right. Hit enter, and you can start placing your pins. Use all the same keys as you did in the Schematic to change rotation, flip the pins etc. Note that the location of the display name is the INSIDE of the pin, as in, the opposite end is the one you'll connect to later.

The pin designator will automatically increment, and if you have numbers in the display name, they will also. You can hit Tab at any time to change the pin display name. Make sure you place the pins in the correct order, and check back with your PCB library footprint if you need to!

Once you have placed all your pins, you'll want to create a little symbol for them. You can access the drawing tools on the toolbar, as displayed by a pencil, ruler and triangle. For most IC's, a simple box is sufficient, so you can use the Draw Rectangle tool to draw a box around your pins. You'll notice that the pins are actually hidden behind the box once you place it - click and drag and select all the pins, then cut and paste them back again. There is probably an easier way to bring them back to the front but I haven't figured it out yet.

Now, one common practice when dealing with larger pin count devices is to switch the pins around to make them a bit easier and cleaner to connect in your schematic, for example grouping all the ground and power pins. You can drag the pins around and place them in any order, as the designator will still remain the same, you are simply changing their visible position.



Now you're done! Save your schematic library.
 
Last edited:

Things

New member
Joined
May 1, 2007
Messages
7,535
Points
0
[size=+2]Creating a schematic[/size]

Now that you have all your component footprints and symbols, you can start creating your schematic. Select your new parts the same way we did earlier and add them to the schematic sheet.

Use the place wire tool and start routing connections! Each wire you place becomes what's known as a "net", so you'll eventually end up with a ground net, a (or multiple) power nets, and various other nets connecting all your components together. Use Esc to cancel placing components or wires.

These nets mean you can also make connections between components without making an explicit connection in your schematic, by setting it's net label. My preferred way of doing this is clicking the Ground symbol in the top right toolbar (the one next to the resistor, not the place part button), and you can select various styles of ports. Before placing them, hit Tab and give them a net name. So for example, if you create 2 "ports" and give them the net name of GND, they will both physically connect when it comes to your PCB design, and also connect to any other nets named "GND".



Now, I was talking about using existing schematic symbols and changing their footprints earlier. Simply create the component footprint in the PCB Library like you did for the others, however don't bother creating anything for it in the Schematic library. Instead, select an existing resistor/capacitor etc in the Altium library. Before placing it, hit Tab, and you will notice once again a Models box on the bottom right. Delete the original footprint, and add your own like you did in the Schematic Library. Take note of the "Edit pins" button in the far left bottom corner of the component properties window, as you may need to use this later.

Now, place the part in your schematic, and you have the default Altium symbol with your custom footprint! Now, to check the pins, hover your mouse over each of the pins. It will bring up a small brown box, with something like Pin R?-2 (2). These last 2 numbers are the pins of the symbol and the component footprint you created. On most resistors and capacitors, this doesn't matter as they aren't polarized, however if you're using a default transistor or diode symbol for example, it does.



If the pin numbers don't match up how you want them, go back into the component properties and click the Edit Pins button. On the left you'll notice the designator of the symbol, and to the right, you'll notice your component footprint name across the top. Doubleclick on the pin you want to change, and change it's designator. Done!

You can change any of the text fields on the symbols by doubleclicking them, however keep all your component designators as R?, C?, U? etc for now.

If you are creating your schematics and realize maybe a pin label is wrong, or it'd be handy if the pin was on the other side of the device, not to worry, simply go back int your Schematic Library and edit it. Once you're done, save the library, then right click up on the component you just updated in the left list of components, and choose "Update schematic sheets".

Check your schematic a few hundred times for errors before you proceed! But don't worry, you can always come back and edit it later into the PCB design.

Once you are happy with your schematic, you can start annotating (or giving components designators). Luckily Altium has a feature to do this built in! Go to Tools -> Annotate Schematics. Select the order of processing of your choice, then hit "Update Changes List", followed by "Accept Changes (Create ECO)".

An ECO is an Engineering Change order - it's basically Altium's way of telling you exactly what it's planning to do, and letting you confirm it's right before you proceed, so in this case you'll see "Modify - R? -> R1", for example. By clicking Validate Changes, Altium checks that there is no conflicts, and you can then accept the changes. All done, all your components now have their own designators!

At this point your schematic is pretty much done. You can export it in various ways such as a .pdf and have other people look over it before you continue if you'd like, or take a screenshot if it's just a small schematic.
 
Last edited:

Things

New member
Joined
May 1, 2007
Messages
7,535
Points
0
Now you have finished your schematic, it's time to transfer it to a PCB! On the tabs along the bottom of the Project panel, select "Files" and you'll be back at the same panel as when you first started. Towards the bottom you will notice a "New from template" dropdown, and at the bottom of this, a "PCB Board Wizard". You may need to minimize a few dropdowns above to see this option.



From here, you can select all your PCB parameters.

Most of the time you'll select a Custom board design, which will bring you to a few options, such as the board size, keepout layer distance etc.

It is a good idea to leave your keepout layer for at least 1mm or so, just to ensure no components or tracks are cut off during manufacturing. I usually deselect "Title block and scale", "Legend String" and "Dimension Lines". Next, select how many layers your board has, for a double layer board I usually select 2 signal layers and 0 power layers. Next select your via types, component types, and also fill in the design rules from your PCB manufacturer.

Note that you can redefine the board shape later, so if you're not sure what final size your board will end up as, just go large and fix it later.

Finish!

Your new PCB will show up under "Free documents", so you will need to drag it into your project, and go ahead and save it.

Next, click Design -> Import Changes from ProjectName, and you will be presented with an ECO once again. Hit validate changes, and check that no errors appear. Sometimes you will get errors such as unable to connect nets or find pins, or bad component designators. Click cancel on the ECO and go back to your schematic, and make sure all your components have proper designators, or re-annotate your schematic, and also check your component pins. Note that pin errors can also cause net errors, even if it doesn't specifically say.

Once you are happy with the ECO, accept the changes, and now all your components will appear in a red box next to the PCB, ready to be placed! This red box is called a "room", and is basically a handy way of separating components if you had multiple sections of a PCB you wanted to group together, for example. However, when you start dragging components onto your PCB, you will notice they show up green, and will give errors if you hover your mouse over them about clearance. This can be resolved by deleting the room.

Unlike most other software, Altium actually runs DRC's (Design rule checks) constantly, so if you try and place a component too close to another, it will give you an error straight away.

Double check that all your components were added to the PCB. If not, it means you've most likely forgotten to add the footprint for it when you were creating it in the Schematic Library. If so, go back to the schematic library, add the footprint, update the part in the schematic, then import changes onto the PCB again. You can also import changes if you need to make changes to your schematics.

If you need to make changes to your component footprints, you can simply access the PCB library again, change the footprint, then rightclick on the component in the list and "Update PCB with ComponentName".

Start dragging your components into position on your PCB, remembering all the usual shortcuts to rotate/flip components. To change the layer of the component, while dragging it, press "l", and it will be flipped to the opposite side of the board.

You can now begin routing the traces on the PCB. Click the "Interactively route connections" button on the toolbar, and click on a component pad you wish to start routing. After clicking, press tab to edit the trace properties. To change the layer of the trace, hit the + or - keys on your numpad. If the existing trace is on the opposite layer, Altium will automatically add a via for you!

You will notice that Altium will automatically prevent you from making connections to other traces or pins not in the same net, so it is important that your clearance constraints are set correctly so Altium knows how far away from other pins and traces to route.

You can edit the design rules at any time from Design -> Rules.

Along the bottom of the workspace, you'll notice tabs for all the various layers of your PCB. Right click on them and you can enable/disable any of them to make routing a bit easier. You can also select which tab you wish to route on, then start routing a connection to start on that layer.

Explore some of the other tool options, such as placing text. If you wish to place an image on your PCB, follow this guide: http://wiki.altium.com/display/ADOH/How+to+import+a+graphic+onto+the+PCB+overlay

Note that with the place pads option, you will need to specify a net in their properties, otherwise Altium will not allow them to connect to anything. This is handy if you want to add testpoints on your PCB without having to create a custom footprint and symbol in your schematic.

*more to come*
 
Last edited:

ARG

Well-known member
Joined
Feb 27, 2011
Messages
6,851
Points
113
Well, I got a license for Altium; going to give this a go, installing it now.

How much is there in the way of pre-made parts and footprints?
I find most of my time in eagle is spent creating footprints and parts. It lacks a lot of SMD IC footprints, SOP, MSOP, SOT ect.

I've heard good things about altium, can't wait to start :D
 
Last edited:

Things

New member
Joined
May 1, 2007
Messages
7,535
Points
0
It has a few, but I think you'll find yourself still making most of them. The upside is Altium has automatic generators for the common parts, everything from chip resistors, MELF packages, to TQFP and DIP. You can find them under the tools window in the PCB editor window.
 

ARG

Well-known member
Joined
Feb 27, 2011
Messages
6,851
Points
113
When's the export PCB part of the guide coming? :)
 

Things

New member
Joined
May 1, 2007
Messages
7,535
Points
0
I'll try remember to whip something up over the weekend - indeed it's not very straightforward :p
 




Top