5V and 3V3 rail with LDO

Schematic
1

Hi,

I am experiencing a weird issue. I have a schematic in which I use a LDO to transform 5V to 3V3. When exporting the schematic to a netlist, the 5V net disappears and becomes connected to 3V3. What could cause this and how can I possibly resolve this?
I have this with the stable version of Kicad 5 for Windows and with the (current) latest nightly (r11234).

Please see the attached image for the schematic of the LDO

V-reg-5V-3V3
V-reg-5V-3V3964Ă—407 4.4 KB

1 Like
2

I don’t see anything specifically wrong with this schematic fragment. So the problem is probably elsewhere on your full schematic. I do have two observations though…

  1. The local labels “+5V” and “+3.3V” are redundant with the global power symbols.
  2. If this passes ERC then you do have your 5V line connected to some other power rail. Unless you changed pin types on the parts from the standard libraries, there is no Power Output type pin to drive the Power Input type pin of the regulator on this schematic fragment.

A highlight net feature in Eeschema would help troubleshoot this, but AFAIK it doesn’t exist.

1 Like
3

There is a highlight net feature in v5 :slight_smile:

Somewhere you have connected the two nets… are you using symbols with hidden power pins by any chance?

The problem is somewhere else, you need to show the whole schematic.

1 Like
4

I quickly tried to find it when writing my message. Apparently I didn’t look close enough…

@xjmaas
To help you find the error, select the following tool:
2018-09-28%2014_25_02-Settings

Then click on your +5V line and all the wires on that net will go form green to magenta. See my example here where I clicked on my VCC net:
2018-09-28%2014_27_00-Eeschema%20%E2%80%94%20KiCad5TestNew%20%5B_%5D%20%E2%80%94%20C__Users_chelliot_Dropbox_RemoteDevelopment_KiCad

This should allow you to quickly find where on your schematic that you might have accidentally connected the +5V to +3V3 nets. (Check the magenta wire areas, ignore the green wire areas.)

Note a couple things about the highlight mode that I just found:

  1. You must click on a wire or wire junction. Clicking on a pin won’t highlight anything, not even the net connected to the pin.
  2. The highlight will stay until you turn it off, even if you change to another tool.
  3. To unhighlight a net click on the schematic anywhere that is not a wire while the highlight net tool is active. If you click on a wire or junction of another net the highlight will move to the newly selected net.
  4. I haven’t figured out if you can have multiple nets highlighted. I suspect not.
  5. Once a net is highlighted, editing it will not change anything remaining on the schematic that is highlighted. If you add wires to the net the added wires will only be green. If you disconnect portions of the net (remove a label, wire segment, etc) everything still existing that was highlighted will still be highlighted.

So, if you use the highlight net tool to find your error, after deleting what you think is the offending connection you will need to switch back to highlight mode and re-highlight your net to see if the change corrected things.

3 Likes
5

I actually have a few symbols using hidden pins, they are 74HC245 from the 74xx library and a 74LVC1G14 from the 74xGxx library which should be connected to the 3.3V powerline and a SST39F040 driven by the 5V line. These are all parts with hidden powerpins.

6

That will be the problem then… if you have mixed voltages for VCC you need to use symbols with explicit power pins.

1 Like
7

@SembazuruCDE,
I do know the highlight function ;). And I have separated the 5V and 3.3V lines deliberately. The only place they are near each other is at the LDO.

8

And, given your conversation with @bobc, on the hidden pins. Given that you are using parts from the standard library with hidden power pins, I suspect that you are using the v4 standard libraries. One of the improvements that was done for the v5 libraries is eschewing the use of hidden pins everywhere except power symbols.

For example, I have the v5 libraries installed and here is the 74HC245 installed on my system (and therefor the one in the v5 standard library):
2018-09-28%2015_07_08-Choose%20Symbol%20(12176%20items%20loaded)

9

I replaced the 74HC245 with the new symbol, but the SST39F040 and 74LVC1G14 are still the legacy symbols? How can I resolved that issue, if at all possible right now?

10

I didn’t even bother to check those two (I only checked the 245). It looks like some bad legacy symbols have slipped through the librarian’s fingers. Understandable given the amount of fixes they had to do, especially since they are all volunteer.

It looks like now is an opportune time for you to learn how to modify an existing symbol for your own use. This is a skill that everyone should learn eventually, the sooner the better. (Often if you have an odd component that you need a symbol for, it is actually faster to create your own symbol than searching the internet for one.) I remember seeing some conversations here about the workflow for modifying an existing symbol to one’s personal libraries, but I don’t have time to search for it. I did scan quickly through the FAQ Index thread, but didn’t see anything stand out. But if you search the forum you hopefully should find help.

It would be nice if you could update these symbols for the librarians (and thus joining the ranks of the Volunteer Librarian Squad, even if only for 2 components). Check out the symbol section of the KLC (KiCad Library Convention) to see what they style guide is. @Rene_Poschl should be able to help point you to the correct resources for contributing. I don’t know if he is the “head” librarian, but he certainly is the most vocal librarian on this forum (thus makes a good POC) that I’ve noticed.

3 Likes
11

@SembazuruCDE

Thanks for the info, I just changed the powerpins of the ST39SF040 (checked the boxes visible and unchecked the boxes for 'Common to all units in symbol) and now the 5V and 3V3 rails are separated.

I’ll try to send an update for the library, but I don’t know if I have the time to do so in the near future…

12

This topic was automatically closed 90 days after the last reply. New replies are no longer allowed.