Altium Designer Schematic Tips & Tricks
By Parker Bondi
September 30, 2024
Below is a list of details that you can add to your schematics to better communicate the intent of the design to the rest of your engineering team. These tips and tricks will make your schematics more useful for the product team, give the PCB Layout Engineer more control over the design, and ensure that the firmware team has the correct information.
1. Add Details About Mating Pairs
For connectors such as battery connectors or board-to-board connectors it is helpful for a designer to add a text frame with the manufacturers part number and manufacturers name of the mating connector that will need to be purchased to connect to your PCB.
Use text frames and tag the component on the schematic by typing P then F and drawing your text frame. Then to tag the component type @ followed by the designator of your component.
This will maintain the reference even if you reannotate your schematics.
2. Use Parameter Sets and Blankets to Define Net Classes
Parameter Sets and Blankets are extremely effective tools deployed in the schematics that I use to create a comprehensive set of PCB design rules. Altium’s PCB design rule checker is a powerful tool that allows a designer to creating custom rules to check for more specific design mistakes that would not be captured by Altium’s default design rules.
For example, here I have created a rule to set the clearance for any object in the net class PDN to 0.178mm.
Here I have created a rule for nets that I wish to route as a 50Ohm impedance trace.
Net classes can also be generated in the PCB but the default settings for Altium designer will over-write your net classes if you make changes to the schematics and import your changes to the PCB layout file.
To add a Parameter Set to your net type P then V then M and click on your nets.
To add a Parameter Set to a group of nets you can use a Blanket. Type P then V then L.
Click and drag the blanket over your nets. Ensure that you blanket fully covers the nets (you can also put it over the net labels if you desire).
Apply a parameter set to the blanket and a Net Class Name and Value.
On the Properties panel click Add and Net Class. Then type in a descriptive Net Class Name in the Values column. I gave this parameter set a Net Class Name parameter with a value of PDN.
Then in your PcbDoc file type D then I to import changes from your schematics.
Click Yes to continue and create the ECO.
You should see that a new net class PDN is being added.
Click Validate Changes and ensure that the green checkmarks come up.
Click Execute Changes and ensure that the second column of green checkmarks come up.
Then click Close.
Then create a design rule for your net class by typing D then R. Right click on the parent level design rule and click New.
Rename your rule. I chose Width_PDN.
And now define the priority of the rule by clicking Priorities.
Altium’s design rules are priority 1 based. This means that when checking the width rule for a track it first checks to see if the priority 1 rule applies to the trace. In this design it checks to see if the Width_50Ohm rule applies. If it does, then Altium stops checking width design rules. If it does not then the design rule checks to see if priority 2 applies followed by priority 3.
3. Color Your Nets
Add color to your nets by typing V and select Set Net Colors then click on the net you would like to color. This will color the net throughout the schematics as well as the PCB.
4. Add A Note With The I2C Address of Each I2C Peripheral
Add a note below your I2C peripheral with the 7-bit address of the component after you have configured the address pins of the device.
I like to use a text frame with the smallest boarder and a Text Margin of 50mil. I draw my schematics on a 100mil grid so when you add a Text Margin of 50mil it nicely centers the text inside the frame.
Make sure to be consistent with the number of bits you use. The datasheet of the temperature sensor shows that when you pull the ADD0 pin to ground the 7-bit address is 1001000 which is 0x48 in hexadecimal.
Get in touch with us
If you’re looking for someone to carefully design your schematics contact us and let us help!