Electronics > Altium Designer

Multi channel design - net classes - isolation between channels

(1/1)

Warhawk:
Guys, I've been working on an HV inverter power stage (3-phase H-bridge). There are 6 isolated drivers in total.
Each driver circuitry is identical. For this reason, I used the multichannel option in altium. This gives me just one schematic page for all 6 drivers.
The problem I face now is related to net classes. I need to set the clearance (isolation) between channels as well as between the low-and high-voltage domain.

Since I have just one schematic page in altium I am not able to define a different class for each channel (like HV1, HV2, HV3...).
I tried the blanket with a parameter set something like Net Class Name - HV$RoomName but it does not work. The compilation does not substitute the parameter.

Does anyone have a clue how to create a Net class with indexes that match the channel?

T3sl4co1l:
Use the other class, schematic or channel whatever it is. :)

Check Project Options/Classes to make sure it's enabled.

Tim

ajb:
Project > Project Options > Class Generation Tab, set the Net Classes dropdown for the sheet to "Local Nets Only" or "All Nets", and you'll get an automatic net class for each sheet instance.  "Local Nets Only" will only add the nets that are fully contained in the sheet, "All Nets" will include the ones that connect off-sheet.  FYI the latter option is not very sophisticated and can end up including power nets in all of the instance classes which may cause issues with rules. 

If you only need to target nets that connect off-sheet (like just the output lines of each driver) then you may be able to do that with a directive or blanket applied at the next sheet level up.  Or just target the compiled net name if it's not too many nets.  You may need to use one of these methods alongside the "Local Nets Only" setting above to get the results you need, depending.

Warhawk:
Fantastic answers guys. This was it!  :-+

Navigation

[0] Message Index