Altium Multi-Channel schematic net labels are not repeated - Page 1
Forum section: electronics / general

author: aslan7
author_rank: Newbie
timestamp: March 29, 2024, 10:53:36 am
content: I am using Altium Designer 20.2.5 and trying to build a hierarchical design. There are two schematics: top level and sub level, as shown in the following figure (named Top Level):What I expected was that all the PWM net names in the sub-level schematic would change properly (PWM1, PWM2...PWM8), but the net names don't change, as shown in the following figure (named SubLevel). Each channel has the same net name.

author: ajb
author_rank: Super Contributor
timestamp: April 01, 2024, 03:57:53 pm
content: Do you get the correct connectivity on the PCB? Altium will show compiled component designators for a multichannel design, but it won't show compiled net names as far as I've seen. So it's not clear that anything is wrong here just from the schematic.

author: aslan7
author_rank: Newbie
timestamp: April 02, 2024, 09:18:19 am
content: I need help what else to check in my project. In ProjectHierarchy.png, my project hierarchy seems okay as far as my understanding. In ComponentDesignators.png, component designators are changing properly; but net labels do not.When I validate my project, I am encountering some errors as shown in Error.png. Also, in PCB side, there's no connection for LED anodes (PCB_Connections.png).I really don't know if something's missed.

author: ajb
author_rank: Super Contributor
timestamp: April 02, 2024, 11:35:38 am
content: It might be because you have a port called "PWM_MCU[1..8]" connected to a bus called "PWM[1..8]". Try setting them to the exact same name. Bus ports are a little weird and I think that may be necessary for them to connect properly.Or it could have something to do with how the PWM_MCU[1..8] port is connected to the next sheet up, can you show that?

author: aslan7
author_rank: Newbie
timestamp: April 02, 2024, 01:07:56 pm
content: I've tried many combinations of port/label naming -including same port and label name- but none of them worked.Previously, the PWM_MCU[1..8] port was not connected anywhere. Now, I removed the port and added a connector and drew the bus; please check if any problem is seen.

author: ajb
author_rank: Super Contributor
timestamp: April 02, 2024, 01:46:26 pm
content: Okay, if PWM_MCU wasn't connected to anything then you seem to be getting correct results. The PCB shows that the PWM nets are resolved to PWM1, PWM2, etc. Again, Altium will NOT show these resolved net names in the schematic, you will only see them on the PCB. Make sure that you have the LEDs actually connected to something and see if it connects properly on the PCB.

author: aslan7
author_rank: Newbie
timestamp: April 03, 2024, 06:25:11 am
content: In the last picture I posted, PWM_MCU nets are connected between the J1 connector and the LEDs. But, on PCB side, they're not connected properly as shown in the following figure.

author: thm_w
author_rank: Super Contributor
timestamp: April 03, 2024, 10:06:56 pm
content: I feel like if you want to use the Repeat options you'd have to repeat the connector itself and not have it connected to a single connector.BUTYou can get this to work fine if you call the port Repeat(PWM_MCU) instead of PWM. Then label the net going in PWM_MCU instead of PWM as you've shown above.

author: nazarevich
author_rank: Newbie
timestamp: November 01, 2024, 02:53:51 am
content: Hi!Try this one.