4
\$\begingroup\$

I have created schematic symbol for a voltage regulator in Altium. It has pin for voltage input and pins for voltage output.

enter image description here

Do I set the electrical type to power for all pins or do I set the vin to Input and Vout to output? I could just set all of them to passive as well. What is the correct way to do this?

\$\endgroup\$
2
  • \$\begingroup\$ Are you wanting to do circuit simulations, or just designing the PCB? \$\endgroup\$
    – JYelton
    Jul 12, 2023 at 22:05
  • \$\begingroup\$ This link will take you to an excellent (and official) Altium forum: live.altium.com/… \$\endgroup\$ Jul 13, 2023 at 12:47

2 Answers 2

3
\$\begingroup\$

When you validate your project the settings in the Connection matrix comes into play:

enter image description here

It can't catch all the errors you make but it might save you from some mistakes. I would set them to Power, then check any warnings I get. If the warnings and errors were just annoying I would set the pins to Passive.

If you want to use theese properties depends on your design environment. If you're a single inexperienced designer, you might want some extra help from the tool. If you are an inexperienced designer in a big team you might waive the ERC warnings and let the review board catch the errors. An engineer with many years of designing might find the Altium settings a nuisance and set everything to Passive because the errors the ERC can check (and generate) doesn't add any value.

Edit: Regarding simulations, I have never used Altium for simulations. At all the places I have worked the simulations have always been done by recreating the circuit in another tool, Hyperlynx, LTSpice etc.

\$\endgroup\$
1
  • \$\begingroup\$ Based on the default table, setting both pins to power should be fine and generate no warnings. \$\endgroup\$
    – jpa
    Jul 13, 2023 at 10:26
1
\$\begingroup\$

If you are only concerned with designing a PCB and not running any circuit simulations within Altium, use Passive for all pins. The electrical rules check (ERC) will consider the pin types and their connections, thus if you don't have other details in place for the simulator, the ERC will generate warnings and/or errors which can become obstacles for simple PCB design.

There are extensions to Altium which will use this information as well, so the real answer is "it depends" based on what you or your company wants to do. For me, I do simulations outside of Altium so almost all of my component library is set up with passive pins (a huge task to fix if we ever decide to change it).

Check the official documentation for more information (though it does not really cover the pin electrical type in any great detail).

\$\endgroup\$
9
  • \$\begingroup\$ I did check the documentation and did not find anything helpful specifically for this query. I thought Altium simulation capabilities are terrible and no one will ever want to use it. \$\endgroup\$
    – quantum231
    Jul 12, 2023 at 22:22
  • \$\begingroup\$ I'm inclined to agree, but there is at least one extension which is useful for checking power dissipation and current versus track widths. I forget the name of it, but at some point I've needed to (as a minimum) specify a few power pins on things. I just don't want my recommendation to lead to heartache later; but I can attest to using "passive" for everything and have completed dozens of successful boards. \$\endgroup\$
    – JYelton
    Jul 12, 2023 at 22:27
  • \$\begingroup\$ ok, just one more thing, since circuits can get quite large and complex I believe we would only ever simulate a small part. This means that we could just recreate that small part of our design in spice and simulate it. Is this how you do it? \$\endgroup\$
    – quantum231
    Jul 12, 2023 at 22:31
  • \$\begingroup\$ @quantum231 Exactly. We simulate portions of circuits as needed, not entire PCB designs. \$\endgroup\$
    – JYelton
    Jul 12, 2023 at 22:48
  • 1
    \$\begingroup\$ @Julien I agree completely! My company requires an ERC directive be set on all unused pins so they will generate a non-connected warning/error if they were not explicitly set to "do not connect" in the schematic. I'd forgotten that we'd set passive and power pins the same (I reverted to installation defaults temporarily to check). \$\endgroup\$
    – JYelton
    Jul 21, 2023 at 17:30

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service and acknowledge you have read our privacy policy.

Not the answer you're looking for? Browse other questions tagged or ask your own question.