Author Topic: Switches on Schematic Do not Create Ratwires on Board  (Read 1705 times)

0 Members and 1 Guest are viewing this topic.

Offline t1d

  • Frequent Contributor
  • **
  • Posts: 602
  • Country: us
Switches on Schematic Do not Create Ratwires on Board
« on: December 13, 2017, 04:32:54 pm »
It seems that net designations, such as power, to not carry through switches.
My schematic is correct and there are no ERC errors. Starting at switch “O/I-1”, pin 2, follow the net to all other connections. Now, look at the board. None of those ratwire/connections exist. Maybe it has to do with the pin output designations of the switch? How to correct, please?
 

Offline hermit

  • Frequent Contributor
  • **
  • Posts: 470
  • Country: us
Re: Switches on Schematic Do not Create Ratwires on Board
« Reply #1 on: December 13, 2017, 05:20:36 pm »
Have you tried to generate a new net list and import it?  This should have nothing at all to do with the power flag.

EDIT:  What is going on with the part of the schematic not shown?  Pins 1 and 8 on U1 are showing a rat?  Did you make the schematic symbol for U1 or was it in the libraries? 
« Last Edit: December 13, 2017, 05:27:17 pm by hermit »
 

Offline Bassman59

  • Super Contributor
  • ***
  • Posts: 1196
  • Country: us
  • Yes, I do this for a living
Re: Switches on Schematic Do not Create Ratwires on Board
« Reply #2 on: December 13, 2017, 05:31:16 pm »
It seems that net designations, such as power, to not carry through switches.
My schematic is correct and there are no ERC errors. Starting at switch “O/I-1”, pin 2, follow the net to all other connections. Now, look at the board. None of those ratwire/connections exist. Maybe it has to do with the pin output designations of the switch? How to correct, please?

A Power Flag is not the same thing as a Power Symbol.

A Power Symbol (the usual sort of VCC or whatever) declares a global net whose name is in the symbol (say VCC) and the one pin in the symbol has an electrical type Power Input. The reason they are Power Inputs is because you'll likely instantiate more than one in a design, and if they were Power Outputs the ERC would give you a "multiple drivers on a net" error. You should use Power Symbols for all of your power-supply rails.

A Power Flag does not give a net any label. Its pin has an electrical type Power Output. It is a trick meant to tell the ERC that, yes, there is a driver (Power Output) on this particular net.

Why is this necessary? Consider: your battery likely has its + and - pins declared as electrical type Power Output. So you can connect them to Power Inputs and ERC is satisfied. (And you can place a Power Symbol, such as GND and VCC, on the battery terminals, which helps to clean up the schematic.) But what about instances where the power input comes from a connector, or is switched as in your case? Pin 2 of your switch is connected to a Power Input (pin 8 of U1A), so without the Power Flag ERC will say "you don't have a driver on your Power net." With the Power Flag in place, as you've done, ERC is satisfied. Assuming that your battery's negative terminal pin is declared as Power Out, the Power Flag on the GND net you've placed at U1A pin 4 is not necessary.

All that said: since your board layout doesn't have silkscreen or any other indication telling us which of the holes are the switch's pins 1, 2 and 3, it's hard to follow what is going on. That U2 is an 8-pin connector isn't helping, either -- are the pins ordered like a DIP/SOIC (increasing down one side then up the other) or are they ordered like a connector (all odd on one side, even on the other)?

Use a text editor to look at the netlist file created by EESchema and verify that the connections are actually there. And, please tell us which version of Kicad you're using. Is it 4.0.7, the latest stable? Is it a nightly build? Is it something older? What canvas are you using (OpenGL or legacy)?
 

Offline t1d

  • Frequent Contributor
  • **
  • Posts: 602
  • Country: us
Re: Switches on Schematic Do not Create Ratwires on Board
« Reply #3 on: December 14, 2017, 09:28:15 am »
Hi, Hermit... Thank you for your help!
Have you tried to generate a new net list and import it?  This should have nothing at all to do with the power flag.
Yes, I know about this required step and I have been doing it correctly, as best I know.

EDIT:  What is going on with the part of the schematic not shown?  Pins 1 and 8 on U1 are showing a rat?  Did you make the schematic symbol for U1 or was it in the libraries?
I have supplied the remainder/complete schematic. The rats on pins 1 and 8 are not connected to switch O/-. I do see why you question them and I will have to figure that out, before production. All of the components are from libraries; I did not make any, for this project.
 

Offline t1d

  • Frequent Contributor
  • **
  • Posts: 602
  • Country: us
Re: Switches on Schematic Do not Create Ratwires on Board
« Reply #4 on: December 14, 2017, 09:55:38 am »
Hi, Bassman... I appreciate your help, greatly!

A Power Flag is not the same thing as a Power Symbol.
Your explanation is good. But, I must admit that I will have to chew on it, to have it sink in permanently. As an example of my lack of understanding, I do not know where to find the power symbol components, too add to the schematic. All of the power components seem to be named as "power flag-symbol(s)." I played with adding the +5V and VDD flags, on both sides of the switch, but this did not create the needed rats.

All that said: since your board layout doesn't have silkscreen or any other indication telling us which of the holes are the switch's pins 1, 2 and 3, it's hard to follow what is going on.
I have added a numbered board, in my reply to Hermit. Let me know, if you need more information.

That U2 is an 8-pin connector isn't helping, either -- are the pins ordered like a DIP/SOIC (increasing down one side then up the other) or are they ordered like a connector (all odd on one side, even on the other)?
The IC is a DIP. I have added the pertinent pins numbers, to the board, in my reply to Hermit.

Use a text editor to look at the netlist file created by EESchema and verify that the connections are actually there.
I have not done this with the text editor, but I have run the ERC and deleted/reconnected the schematic wires, several times. I will look, with the editor.

And, please tell us which version of Kicad you're using. Is it 4.0.7, the latest stable? Is it a nightly build? Is it something older? What canvas are you using (OpenGL or legacy)?
I am using v4.0.7. The board is in the default view. I am not sure where to look for the OpenGL/Legacy info? I did not, intentionally, change it from the default.

I will say this. This board is the third iteration of this project; all boards have used the same schematic. When I built this board, I had difficulty moving the components and had to use the Cairo canvas, to get things in place. I found this odd.
 

Offline t1d

  • Frequent Contributor
  • **
  • Posts: 602
  • Country: us
Re: Switches on Schematic Do not Create Ratwires on Board
« Reply #5 on: December 14, 2017, 10:07:50 am »
Bassman,
I opened the netlist in Note Pad. I have not worked with the netlist, in the editor, enough to be able to read it very well. But, it does not look like the connections were made, to me. Again, this is probably a bit above my pay grade. I have attached the Note Pad file, for your review. Thank you, so much, for your efforts.
 

Offline donotdespisethesnake

  • Frequent Contributor
  • **
  • Posts: 859
  • Country: gb
  • Embedded stuff
Re: Switches on Schematic Do not Create Ratwires on Board
« Reply #6 on: December 14, 2017, 11:06:47 am »
The netlist looks ok, but the reference designators on the PCB don't appear to match the schematic. You might have orphaned footprints.

When you import netlist to pcbnew, set "Exchange footprint" to "Change", and "Extra footprints" to "Delete". That will ensure the pcb matches your schematic. Also pay careful attention to messages in the Messages window.
Bob
"All you said is just a bunch of opinions."
 

Offline t1d

  • Frequent Contributor
  • **
  • Posts: 602
  • Country: us
Re: Switches on Schematic Do not Create Ratwires on Board
« Reply #7 on: December 14, 2017, 03:03:28 pm »
Thanks, DDTS, that was the cure! Lesson learned... maybe...
 

Offline hermit

  • Frequent Contributor
  • **
  • Posts: 470
  • Country: us
Re: Switches on Schematic Do not Create Ratwires on Board
« Reply #8 on: December 14, 2017, 04:47:38 pm »
I was on the right track, wrong view. ;)  I'm so automatic about making those changes when I import the netlist I don't know what it looks and what problems it solves when you don't do it.
 

Offline Bassman59

  • Super Contributor
  • ***
  • Posts: 1196
  • Country: us
  • Yes, I do this for a living
Re: Switches on Schematic Do not Create Ratwires on Board
« Reply #9 on: December 14, 2017, 06:10:25 pm »
The netlist looks ok, but the reference designators on the PCB don't appear to match the schematic. You might have orphaned footprints.

When you import netlist to pcbnew, set "Exchange footprint" to "Change", and "Extra footprints" to "Delete". That will ensure the pcb matches your schematic. Also pay careful attention to messages in the Messages window.

That probably explains the oddball footprints.
 

Offline Bassman59

  • Super Contributor
  • ***
  • Posts: 1196
  • Country: us
  • Yes, I do this for a living
Re: Switches on Schematic Do not Create Ratwires on Board
« Reply #10 on: December 14, 2017, 07:32:35 pm »
Hi, Bassman... I appreciate your help, greatly!

A Power Flag is not the same thing as a Power Symbol.
Your explanation is good. But, I must admit that I will have to chew on it, to have it sink in permanently. As an example of my lack of understanding, I do not know where to find the power symbol components, too add to the schematic. All of the power components seem to be named as "power flag-symbol(s)." I played with adding the +5V and VDD flags, on both sides of the switch, but this did not create the needed rats.

The power symbols are in the same library as the Power Flag, power.lib. They're all given obvious names, like VCC and VDD and GND and +12V and such. In the right-hand toolbar, click the ground symbol ("place power port") and the power symbol library should open. Or just click the op-amp symbol ("place component") and choose the power library. If you do not see the power library listed when you click on place component, go to your Preferences => Component Libraries menu item, and in the dialog that pops up, make sure power is listed in the top box. If it is not, you must add it; it should be in the same directory as all of the other default Kicad libraries.

That U2 is an 8-pin connector isn't helping, either -- are the pins ordered like a DIP/SOIC (increasing down one side then up the other) or are they ordered like a connector (all odd on one side, even on the other)?
The IC is a DIP. I have added the pertinent pins numbers, to the board, in my reply to Hermit.[/quote]

If it's a DIP, it won't fit into that footprint!

And, please tell us which version of Kicad you're using. Is it 4.0.7, the latest stable? Is it a nightly build? Is it something older? What canvas are you using (OpenGL or legacy)?
I am using v4.0.7. The board is in the default view. I am not sure where to look for the OpenGL/Legacy info? I did not, intentionally, change it from the default.[/quote]

From the top pcbnew menu, choose "View," and at the bottom you'll see three "canvas" options: Legacy, OpenGL and Cairo. OpenGL is the new thing, and has a few features not in Legacy, such as the push-and-shove router (a work of genius) and differential pair support. At some point, once all of the features in the Legacy canvas are implemented in OpenGL, Legacy will go away.
 


Share me

Digg  Facebook  SlashDot  Delicious  Technorati  Twitter  Google  Yahoo
Smf