Hi there! Last time has been worked a lot with my Arduino Nano clone. I has a EAGLE 9 prototyping environment installed, so I have edited those files in this workspace. When I try to connect .brd with .sch, there is a lot of errors becomes visible and I have no idea how to fix them. Can't figure out this problem. Any help is much appreciated!
Mihail, please post the ERC error list.
Sorry, can't figure out how to change language in EAGLE. Just tried to search, but nothing found. So, there is an image, but in Russian: https://imgur.com/a/D0OjgEW It is a "Consistency errors", like "Part U$36 not found in the board" and "Only INPUT pins on circuit..."
Mihail P. wrote: > like "Part U$36 not found in the board" Is there a part U$36 in the board? Mihail Podivilov wrote: > When I try to connect .brd with .sch, Why and how did you split them? You learned a important thing: never edit a *.brd without having opened the corresponding *.sch!
: Edited by Moderator
It is too difficult for me to understand what is the U$36 part in the circuit. I just modified the existing .brd / .sch, presented by gravitech.us (original .sch & .brd atttached to this message in zipped archive). Can you help me to figure out what is the problem? When I try to edit original .sch/.brd, there is also those errors are apperas, even if I don't modified nothing. Thanks!
Mihail Podivilov wrote: > Can't figure out this problem. Simply delete the Logo in your .sch and you are done. Then keep in mind, to work with projects and always open .sch AND .brd when you are working with Eagle. So Eagle can hold both files in a consistent state, that means, that there are no substantial differences between them. You had inserted some "logo" in your Schematics and this got the number U$36. W.S.
Thanks, it worked. But I still have a lot of errors (like a "Only INPUT pins on circuit N$12", "Only INPUT pins on circuit N$13", etc. And a lot of warnings, such as "NC pin U2 NC1 connected to N$14", "Only one pin in circuit N$27", etc. What should I do right now? Thanks!
Mihail P. wrote: > What should I do right now? Thanks! Ignore them, the designer uses maybe testpoints instead of pins so eagle sees only one connection in the net. Additional there are only inputs on this nets. Others are missing junctions, you can add them with the junction command.
Welp. Thanks! Another one question is how to order assembly of this PCB? I heard about multiple sites where I can do that, but help me to choose the right way in my situation. I need to assembly up to 5 prototypes of them, so where can I find the site to simply provide electrical scheme (.sch) and board (.brd), then get a my produced board?
HyperMario wrote: > Others are missing junctions, you can add them with the junction command. Can you give me an example how can I do this in proper way?
: Edited by User
Mihail P. wrote: > Can you give me an example how can I do this in proper way? Type JUN and put the green dot on the junctions where eagle claims the missung junction
HyperMario wrote: > Type JUN and put the green dot on the junctions where eagle claims the > missung junction Ok, done that. So, there are still 35 ERC warnings...
Mihail P. wrote: > I find the site to simply provide electrical scheme (.sch) and board > (.brd), then get a my produced board? You only have to send the .brd file. There are lots of it, depends where you live. See here: https://www.mikrocontroller.net/articles/Platinenhersteller
Mihail P. wrote: > Ok, done that. So, there are still 35 ERC warnings... There are all OK. The warnings are mostly different supply name between net and pin. That's quite normal. The errors depends on the designers intention to explicitly show that unconnected pins means unconnected pins. He made a NC (not connected) device to show that. Good idea i think.
Many thanks, HyperMario! It is all OK right now. I will try to order a circuit board assembly later.
Mihail P. wrote: > I will try to order a circuit board assembly later. Maybe it's easier to buy a nano directly.
HyperMario wrote: > Maybe it's easier to buy a nano directly. Sure, but I want to understand how prototyping and final production take place. :) As a programmer, I also want to create special software to ease the programming learning in our college.
Mihail P. wrote: > Sure, but I want to understand how prototyping and final production take > place. :) Maybe you should consider a manufacturer where you get the stencil too. Using solder cream (and a pizza reflow oven) is way nearer SMD production than using a solder iron.
Hey, just figured out that jlcpcb.com is what I need. I has generated gerber files (CAM data), but I want a real working prototype, not only the PCB. I don't need to solder myself :) Isn't .sch file is intended for data specification, such as AVR chip info and same? I want to assembly a board with all components on them, not only the board to solder later.
Mihail P. wrote: > I want to assembly a board with all components on them, > not only the board to solder later. The pcb manufacturer needs the .brd file (or gerber and drill file). Gerber is - let's say - not easy and error prone. You always have to check with a viewer before production. Manufacturing a complete board requires a BOM (bill of material). Normally you have to specify all parts (except standard like resisitors) with a unique MPN (manufacturer product number).
It's pretty hard, huh? For example, I has ATMEGA168-20AU specified in .sch file (and such). Is it not enough?
Just ordered 10 pcs of PCB prototypes. Good luck to me! Will try to find somebody who can assembly the details in my country :) And, as always, thanks!
Mihail P. wrote: > I has ATMEGA168-20AU specified in > .sch file (and such). Is it not enough? The schematicic holds the information, I dont know if it's complete You can build the BOM with the "run bom" command Due to this design https://www.rs-online.com/designspark/reference-design-of-arduino-nano-3-0 it's an ATMEGA328P-AU, there is the rest of the BOM too and RS has branches in several countries
Thanks! Works like a charm.
Mihail P. wrote: > But I still have a lot of errors (like a "Only INPUT pins on circuit > N$12", "Only INPUT pins on circuit N$13", etc. > > What should I do right now? Thanks! You always should understand the schematics and how it is intended to work. When you have only inputs on a net, then WHO drives this net? Did you forget to connect it to the output of a chip? Messages like "Pin V+ connected to Vcc" or so are usually neglible, but check them carefully and decide by yourself, if this is OK. A bit more harmful are situations, where suppy-pins of some chips are not directly shown in the schematics. Best example is a SN7400 (4 nands). Placing it in the schematics you will get all 4 gates, but the supply connectiosn GND and VCC are usually hidden and automatically connected to the rails GND and VCC - if they exist! So the better way is, to invoke those supply items with the invoke function and connect them by yourself to that rails you want them to be connected. The ERC can halp you to detect design failures of such kinds, so do not IGNORE them, but rather check them, if they are neglible or not. W.S.