Update Using Altium authored by Alia Peterson's avatar Alia Peterson
# Altium’s Layout:
- Projects column - left side column - interact with your existing files and make new ones here
- Panels button - bottom right corner - this has the panel options which will pop up on the right side of the screen when you click on them
- Top ribbon - includes things like File, Edit, View. This will be where you find some tools
- Main workspace - Middle of the screen - where you interact with components, and create your design
- Workspace top ribbon - Top of the workspace, a little floating ribbon with buttons that help you build your circuits. Go here when you want to wire or route things or place text.
- Properties panel - If you click on a component and click enter, it will usually open the properties panel where you can edit the component and rename the part and any pins or other things.
## Making a New Project:
1. Make a new project - File >> New >> Project
1. Make a new schematic file and a new PCB file inside your project (Right click your project in the left panel)
<details><summary>Steps for the Schematic Document:</summary>
1. To place components - open your schematic file, click on the panels button and select Components.
1. Choose WarnickShareLibrary.SchLib - "J:\groups\warnickshare\AltiumLibraryAndRules\WarnickShareLibrary.SchLib"
1. (If you don't see this library, click the three lines on the right, then click on Libraries Preferences then Add Library and add the library.)
1. Now you can select the schematic library in the pull down options.
1. Search for the components you need and place them by dragging them onto the schematic or by right clicking on their name and clicking the “Place” option. You can then click Tab to open the properties panel and edit the pin names and designators and comment before placing the component.
1. To change the pin names or designators, click on Pins at the top of the Properties panel, then click on the little pencil at the bottom of the Pins section
1. Pin Names are what you want to call the pin - like a word describing what that pin is for (Ex. GND for ground). Pin Designators are numbers, so you can number the pins.
Once you have all your components on the schematic, you can connect them using the place wire button on the top ribbon.
1. Place Net Labels - Under Place (top ribbon), select Net Label. Click Tab to edit the net name. Click on the wire you want to name to leave the Net Label there. These are super important! They help establish connections between items. You also need them to do things like differential pair routing.
1. To place a ground net, click the little red triangle in the workspace ribbon. Be sure to label everything properly.
</details>
<details><summary>Steps for PCB Document:</summary>
1. Once your schematic is finished, switch to the PCB document. In this document, there are three different ways to view the board.
- If you type the number “1”, you will be able to edit the board shape with options under Design
- If you type 2 - this is where you will be routing and moving components around - the majority of your work will be done here for the PCB. In this setting, the board is black and the components will likely be colorful.
- If you type 3, you will be able to see your board in the 3d view.
1. Click on Design - Import changes from schematic - this will import the things you did in the schematic document.
1. You can move the components around to arrange them how you like - push space when you’re dragging it around to make the components rotate.
1. Connect the components with traces - Interactively Route Connections button (looks like a little line with two holes on the ends) on the ribbon on the top of the screen
1. When routing, rotate through the corner options by using shift+space. You want your traces to not have any super sharp corners - We typically want to use the 45 degree curves or 90 degree curves - the curves, not the corners. We want wider curves when possible.
- When routing, you can hit space to make the route turn the other direction.
- You can adjust the corners manually by clicking on the corners and dragging them where you want them.
1. Importing layer stack - Open the layer stack manager under Design. Then click File > Load Stackup From File.
1. Go to the LayerStackFiles folder through the following file path: "J:\groups\warnickshare\AltiumLibraryAndRules\LayerStackFiles" J stands for J Drive. Your J Drive will be called something like your_username (\\fs-caedm)(J:) in your file explorer.
1. Select either OSHPark - 2 layers or OSHPark - 4 layers depending on what you’re doing. 4 layers is a good bet. Save this file.
1. To resize your board, type the number 1, then click Design at the top, and then Edit Board Shape. Drag the sides of the board to the size you want.
1. Polygon manager - Tools > Polygon Pours > Polygon Manager
1. To make a ground plane - click on the “New Polygon from…” button. Then choose Board Outline - this will create a plane across your whole board.
1. On the right side panel of the polygon pour manager, you can change the net of the new polygon to ground - it should be one of the options under Net.
1. Repeat steps 10 and 11 again for as many layers as you have in your board - so in a 4 layer board, you will have four ground layers. For each polygon pour, adjust the Layer on the right, you need one ground plane for each layer of the board (L1, L2, etc.). You can also adjust the name of the polygon on the right side panel.
1. Go to Design Rules. Under Plane, PolygonConnect, change the connect style to Direct Connect.
1. Click apply and OK
1. The board may be bright red, or look strange. Open up Tools, highlight over Polygon Pours and click on Shelve to hide these polygons. Always remember to repour your polygons by clicking on repour all under Tools >> Polygon Pours. You can also restore your shelved polygons.
</details>
<details><summary>How to make a new component:</summary>
1. Look at the datasheet for the component you want to build - it should have recommendations on how to make a footprint for it - including dimensions
1. Open the warnickshare pcb library and click Add in the left side panel
1. Place a pad - Under Place in the Top Ribbon
1. Open the properties panel - change the layer to the Top Layer
1. In the Pad Stack section, change the shape for the top layer to rectangle.
1. Adjust the size to reflect the datasheet’s diagram or description for the footprint.
- When making a component footprint, if you need to place several pads, you can Copy + Paste it onto itself, click edit, move (x, y) to translate it. This helps with getting the measurements right.
1. Add a little dot to indicate which direction to put the chip down. Just Place a circle, you can change the size.
To make a new symbol:
1. Open the warnickshare schematic library
1. Place pins and shapes until you get something that represents your part. It doesn’t really matter too much what your schematic component looks like.
1. When placing pins, you want the numbers closer to the body of your symbol, the + on the other side should be on the outside.
1. You connect it to your footprint by selecting Add Footprint at the bottom of the page and Browse until you find the footprint you want to connect it to.
1. Select Pin Map to make sure your pins are lined up correctly with the footprint.
</details>
<details><summary>Finishing Touches:</summary>
- Traces:
- Sometimes you want to use thicker traces. You may want to use this when the trace is for power - like connecting 3.3V or 5V. To change the width of the traces in PCB mode, select the trace you want to edit, then click Tab to make sure it selects the entire trace. Next, open the Properties panel on the right and change the Width (under Properties section) to the size you want (20mil is a good option).
- No sharp corners
- Design rules:
These rules are what the computer uses to judge whether your board is valid or not. The built in rules are fine for some things, but you can adjust these rules when you need to. If you have colorful parts that have little messages or numbers on them, you likely are breaking a design rule.
- Click on Design, then Rules to access the rules
- If you want to assign your differential pair to a class, go to Design, then Classes
- Go down to Differential Pair Classes, then add a new class.
- Select the pair you want to put into this class (the pair name is the word in the nets on the diff pairs before the _P and _N)
- Click the >> button to put it into this class
- Clearance Rules - these set how much clearance you want to give different components (like space between a route and a pad). Under Clearance Rules, select the Ignore Pad to Pad clearances within a footprint. This will clear up if there is a clearance error within a component
- Under Differential Pairs Routing - make your rule where the object matches Diff Pair Class then the name of your diff pair class or All Differential Pairs
- Differential Pair routing:
Sometimes you need to have routes that are the same length to preserve the signal that passes through it.
To do this:
- In your schematic file, click Place, highlight over Directives, and select Differential Pair.
- Click on the two wires you want to be a differential pair - have the same length - this will leave a little red symbol on each of them.
- Click on the red icons and make sure the labels are the same as each other
###Rename the two wires with nets so they have the same name (probably just the label name) with one having an underscore N and the other with an underscore P (for negative and positive) Ex. RF_N and RF_P
- Save the schematic, open the PCB file, and import the changes
- Change the routing option to Interactive Differential Pair Routing (You can change this through the
- Workspace Ribbon or through the Route button at the top
- You can try different corner types here as well until you find one that looks good by using shift + space.
- Click on one of the pads you want to route from and it should automatically start routing the other one too. Connect to the end pad and it should create two traces close together.
- Check to make sure the two traces are the same length by hovering over the traces and it should show that they are the same or very, very close to the same length.
- Adjusting differential pairs if one route is shorter than the other:
- Under Route, choose interactive length tuning, hit tab and select accordion on the right.
- Click the shorter route on a space with a long straight area. Move your mouse to the right and it should start making adjustments to the route.
- Adjust the route on the right by changing the altitude (how high or low it goes) and radius (how far apart the curves are). Choose the rounded option style.
- Making the holes all over the board (Via stitching):
This connects the grounds to each other and catches any stray electric fields.
1. Repour your polygons
1. Tools > Via Stitching/Shielding > Add Stitching to Net
1. Change the Net to GND
1. Change the Grid to whatever you want, somewhat often, but not all over the place - maybe like 200mil.
1. You can also adjust the size of the holes - Diameter 35mil, hole size 25mil is a good size
- Making little holes in a certain spot on the board - like around the SMA input:
1. Repour your polygons
1. Tools > Via Stitching/Shielding > Add Shielding to Net
1. Change the Net to whatever net you want to shield
1. Change the Grid to whatever you want, somewhat often, but not all over the place - maybe like 30 mil.
1. You can also adjust the size of the holes - Diameter 25mil and hole size 15mil is a good size.
- If you don't want the top solder on the copper traces, add polygons to the Top Solder layer covering those traces. You can repour them in their properties panel. You can just Place a polygon on the board and draw it where you want it.
- Add lines on mechanical 1 layer around the outside of the board
</details>
<details><summary>Tips and Tricks:</summary>
- Naming a part - Designator can be information like "Balun" or "3V". Naming pins - designator is number, name is a name.
- To find a library that you've opened, click on the bottom left - SCH Library
- Push space while dragging a component or net label to make it rotate.
- When saving things, the little red file symbol on the left in the projects panel turns gray.
- Navigating 3d mode:
- Hold down shift and drag with right click to rotate the board to view from different angles
- Click 0 to orient the board horizontally (rotated 0 degrees)
- Click 9 to orient the board vertically (rotated 90 degrees)
- Click 8 to orient the board from the house view.
- Changing the size of the grid - Type “g” to change the grid size
- Switch between measurement units - type “q”. We prefer mil (1000th of an inch) over mm.
- You can see which one you’re currently using by looking to the bottom left where it describes the grid and the dimensions and units.
- You can keyboard shortcut into the menus and options by typing the underlined letter
- Ctrl + scroll in and out to zoom in and out
- Right click drag to move the board around
- To measure - Ctrl m
- To clear measurements - Shift c
- In the pcb view, click shift-s to change what you see
- Click Tab after selecting part of the trace to select all of that trace
# Altium’s Layout:
- Projects column - left side column - interact with your existing files and make new ones here
- Panels button - bottom right corner - this has the panel options which will pop up on the right side of the screen when you click on them
- Top ribbon - includes things like File, Edit, View. This will be where you find some tools
- Main workspace - Middle of the screen - where you interact with components, and create your design
- Workspace top ribbon - Top of the workspace, a little floating ribbon with buttons that help you build your circuits. Go here when you want to wire or route things or place text.
- Properties panel - If you click on a component and click enter, it will usually open the properties panel where you can edit the component and rename the part and any pins or other things.
## Making a New Project:
1. Make a new project - File >> New >> Project
1. Make a new schematic file and a new PCB file inside your project (Right click your project in the left panel)
<details><summary>Steps for the Schematic Document:</summary>
1. To place components - open your schematic file, click on the panels button and select Components.
1. Choose WarnickShareLibrary.SchLib - "J:\groups\warnickshare\AltiumLibraryAndRules\WarnickShareLibrary.SchLib"
1. (If you don't see this library, click the three lines on the right, then click on Libraries Preferences, click project at the top, then Add Library and add the library.)
1. Now you can select the schematic library in the pull down options.
1. Search for the components you need and place them by dragging them onto the schematic or by right clicking on their name and clicking the “Place” option. You can then click Tab to open the properties panel and edit the pin names and designators and comment before placing the component.
1. To change the pin names or designators, click on Pins at the top of the Properties panel, then click on the little pencil at the bottom of the Pins section
1. Pin Names are what you want to call the pin - like a word describing what that pin is for (Ex. GND for ground). Pin Designators are numbers, so you can number the pins.
Once you have all your components on the schematic, you can connect them using the place wire button on the top ribbon.
1. Place Net Labels - Under Place (top ribbon), select Net Label. Click Tab to edit the net name. Click on the wire you want to name to leave the Net Label there. These are super important! They help establish connections between items. You also need them to do things like differential pair routing.
1. To place a ground net, click the little red triangle in the workspace ribbon. Be sure to label everything properly.
</details>
<details><summary>Steps for PCB Document:</summary>
1. Once your schematic is finished, switch to the PCB document. In this document, there are three different ways to view the board.
- If you type the number “1”, you will be able to edit the board shape with options under Design
- If you type 2 - this is where you will be routing and moving components around - the majority of your work will be done here for the PCB. In this setting, the board is black and the components will likely be colorful.
- If you type 3, you will be able to see your board in the 3d view.
1. Click on Design - Import changes from schematic - this will import the things you did in the schematic document.
1. You can move the components around to arrange them how you like - push space when you’re dragging it around to make the components rotate.
1. Connect the components with traces - Interactively Route Connections button (looks like a little line with two holes on the ends) on the ribbon on the top of the screen
1. When routing, rotate through the corner options by using shift+space. You want your traces to not have any super sharp corners - We typically want to use the 45 degree curves or 90 degree curves - the curves, not the corners. We want wider curves when possible.
- When routing, you can hit space to make the route turn the other direction.
- You can adjust the corners manually by clicking on the corners and dragging them where you want them.
1. Importing layer stack - Open the layer stack manager under Design. Then click File > Load Stackup From File.
1. Go to the LayerStackFiles folder through the following file path: "J:\groups\warnickshare\AltiumLibraryAndRules\LayerStackFiles" J stands for J Drive. Your J Drive will be called something like your_username (\\fs-caedm)(J:) in your file explorer.
1. Select either OSHPark - 2 layers or OSHPark - 4 layers depending on what you’re doing. 4 layers is a good bet. Save this file.
1. To resize your board, type the number 1, then click Design at the top, and then Edit Board Shape. Drag the sides of the board to the size you want.
1. Polygon manager - Tools > Polygon Pours > Polygon Manager
1. To make a ground plane - click on the “New Polygon from…” button. Then choose Board Outline - this will create a plane across your whole board.
1. On the right side panel of the polygon pour manager, you can change the net of the new polygon to ground - it should be one of the options under Net.
1. Repeat steps 10 and 11 again for as many layers as you have in your board - so in a 4 layer board, you will have four ground layers. For each polygon pour, adjust the Layer on the right, you need one ground plane for each layer of the board (L1, L2, etc.). You can also adjust the name of the polygon on the right side panel.
1. Go to Design Rules. Under Plane, PolygonConnect, change the connect style to Direct Connect.
1. Click apply and OK
1. The board may be bright red, or look strange. Open up Tools, highlight over Polygon Pours and click on Shelve to hide these polygons. Always remember to repour your polygons by clicking on repour all under Tools >> Polygon Pours. You can also restore your shelved polygons.
</details>
<details><summary>How to make a new component:</summary>
1. Look at the datasheet for the component you want to build - it should have recommendations on how to make a footprint for it - including dimensions
1. Open the warnickshare pcb library and click Add in the left side panel
1. Place a pad - Under Place in the Top Ribbon
1. Open the properties panel - change the layer to the Top Layer
1. In the Pad Stack section, change the shape for the top layer to rectangle.
1. Adjust the size to reflect the datasheet’s diagram or description for the footprint.
- When making a component footprint, if you need to place several pads, you can Copy + Paste it onto itself, click edit, move (x, y) to translate it. This helps with getting the measurements right.
1. Add a little dot to indicate which direction to put the chip down. Just Place a circle, you can change the size.
To make a new symbol:
1. Open the warnickshare schematic library
1. Place pins and shapes until you get something that represents your part. It doesn’t really matter too much what your schematic component looks like.
1. When placing pins, you want the numbers closer to the body of your symbol, the + on the other side should be on the outside.
1. You connect it to your footprint by selecting Add Footprint at the bottom of the page and Browse until you find the footprint you want to connect it to.
1. Select Pin Map to make sure your pins are lined up correctly with the footprint.
</details>
<details><summary>Finishing Touches:</summary>
- Traces:
- Sometimes you want to use thicker traces. You may want to use this when the trace is for power - like connecting 3.3V or 5V. To change the width of the traces in PCB mode, select the trace you want to edit, then click Tab to make sure it selects the entire trace. Next, open the Properties panel on the right and change the Width (under Properties section) to the size you want (20mil is a good option).
- No sharp corners
- Design rules:
These rules are what the computer uses to judge whether your board is valid or not. The built in rules are fine for some things, but you can adjust these rules when you need to. If you have colorful parts that have little messages or numbers on them, you likely are breaking a design rule.
- Click on Design, then Rules to access the rules
- If you want to assign your differential pair to a class, go to Design, then Classes
- Go down to Differential Pair Classes, then add a new class.
- Select the pair you want to put into this class (the pair name is the word in the nets on the diff pairs before the _P and _N)
- Click the >> button to put it into this class
- Clearance Rules - these set how much clearance you want to give different components (like space between a route and a pad). Under Clearance Rules, select the Ignore Pad to Pad clearances within a footprint. This will clear up if there is a clearance error within a component
- Under Differential Pairs Routing - make your rule where the object matches Diff Pair Class then the name of your diff pair class or All Differential Pairs
- Differential Pair routing:
Sometimes you need to have routes that are the same length to preserve the signal that passes through it.
To do this:
- In your schematic file, click Place, highlight over Directives, and select Differential Pair.
- Click on the two wires you want to be a differential pair - have the same length - this will leave a little red symbol on each of them.
- Click on the red icons and make sure the labels are the same as each other
###Rename the two wires with nets so they have the same name (probably just the label name) with one having an underscore N and the other with an underscore P (for negative and positive) Ex. RF_N and RF_P
- Save the schematic, open the PCB file, and import the changes
- Change the routing option to Interactive Differential Pair Routing (You can change this through the
- Workspace Ribbon or through the Route button at the top
- You can try different corner types here as well until you find one that looks good by using shift + space.
- Click on one of the pads you want to route from and it should automatically start routing the other one too. Connect to the end pad and it should create two traces close together.
- Check to make sure the two traces are the same length by hovering over the traces and it should show that they are the same or very, very close to the same length.
- Adjusting differential pairs if one route is shorter than the other:
- Under Route, choose interactive length tuning, hit tab and select accordion on the right.
- Click the shorter route on a space with a long straight area. Move your mouse to the right and it should start making adjustments to the route.
- Adjust the route on the right by changing the altitude (how high or low it goes) and radius (how far apart the curves are). Choose the rounded option style.
- Making the holes all over the board (Via stitching):
This connects the grounds to each other and catches any stray electric fields.
1. Repour your polygons
1. Tools > Via Stitching/Shielding > Add Stitching to Net
1. Change the Net to GND
1. Change the Grid to whatever you want, somewhat often, but not all over the place - maybe like 200mil.
1. You can also adjust the size of the holes - Diameter 35mil, hole size 25mil is a good size
- Making little holes in a certain spot on the board - like around the SMA input:
1. Repour your polygons
1. Tools > Via Stitching/Shielding > Add Shielding to Net
1. Change the Net to whatever net you want to shield
1. Change the Grid to whatever you want, somewhat often, but not all over the place - maybe like 30 mil.
1. You can also adjust the size of the holes - Diameter 25mil and hole size 15mil is a good size.
- If you don't want the top solder on the copper traces, add polygons to the Top Solder layer covering those traces. You can repour them in their properties panel. You can just Place a polygon on the board and draw it where you want it.
- Add lines on mechanical 1 layer around the outside of the board
</details>
<details><summary>Tips and Tricks:</summary>
- Naming a part - Designator can be information like "Balun" or "3V". Naming pins - designator is number, name is a name.
- To find a library that you've opened, click on the bottom left - SCH Library
- Push space while dragging a component or net label to make it rotate.
- When saving things, the little red file symbol on the left in the projects panel turns gray.
- Navigating 3d mode:
- Hold down shift and drag with right click to rotate the board to view from different angles
- Click 0 to orient the board horizontally (rotated 0 degrees)
- Click 9 to orient the board vertically (rotated 90 degrees)
- Click 8 to orient the board from the house view.
- Changing the size of the grid - Type “g” to change the grid size
- Switch between measurement units - type “q”. We prefer mil (1000th of an inch) over mm.
- You can see which one you’re currently using by looking to the bottom left where it describes the grid and the dimensions and units.
- You can keyboard shortcut into the menus and options by typing the underlined letter
- Ctrl + scroll in and out to zoom in and out
- Right click drag to move the board around
- To measure - Ctrl m
- To clear measurements - Shift c
- In the pcb view, click shift-s to change what you see
- Click Tab after selecting part of the trace to select all of that trace
</details>
\ No newline at end of file