Go Down

Topic: Schematic Check Needed Please. (Read 2034 times) previous topic - next topic

CrossRoads

"double-line thing"
You can select View:Layers. and deselect the Unrouted layer, they will stop appearing.
Or click the Rats Nest button (lower left, looks like an X), that will connect traces to the nearest components.
Designing & building electrical circuits for over 25 years.  Screw Shield for Mega/Due/Uno,  Bobuino with ATMega1284P, & other '328P & '1284P creations & offerings at  my website.

winner10920

Usually(in kicad atleast) those lines are just for you to see what goes where, to help place components for easy routing
I think you can disable/hide it with a button or setting
id look over the whole thing but unfortunately kicad can't open eagle files

xl97

hi guys...

thanks for the replies..

(Crossroads - you get my emails last night/today?)

Im not sure what RatsNest will do?  connect to nearest component?

I was toggling the unrouted layer.. but was curious as to why say resistor A would have 3 lines going to cap B for example..

I would understand 1 line to each side of the resistor/cap.. but why would one side have 2 lines going to one side of the cap  (just a general example of what i was seeing)..

it lead me second guess myself.. and think the schematic portion was incorrect (which is was.. but not showing multiple lines..etc)


anyways.. here is my second iteration of a SMD based Arduino circuit with uSD socket on board.. (maybe similar to a pro-mini or something with uSD on bottom)

(still have found an Eagle part for the level converter)..

feed back on the schematic (if things are wrong.. or better things to do/document?)... 

as well as how realistic setting up a board like this would be..

thanks!



xl97

Here is another version.. (latest attempt..LOL)

I believe I have found the leveer converter chip/package for eagle..

(I hope I hooked it up correctly)??

I 'think' I have thing the schematic correct? (if anyone can verify?)

I have the PCB dimensions.. and my parts positioned on the stage..

and thats about as far as I am!..

learning alot.. getting more comfortable using Eagle.. finding/using/re-using parts..others schematics.etc..
(the library/add still kills me to find anything!)

What is next?

I believe I have also correct/fixed all warnings and errors given when in the schematic editor as well!..

Do I click on the auto-route button next or something?


thanks for looking and feedback is appreciated!

take care!

CrossRoads

I got the files, but not until after midnight. Went to bed shortly after.

SMDuino, looks like normal unrouted board to me. All the criss-cross lines are an indication that your parts placement needs adjsuting.
You want to minimize those, or will have a hard time getting it all connected. Reassigning IO to the connector pins may help there.

The signals on the ICSP connector are not correct - you need SCK (D13), MISO, MOSI there. The Green names do not make the connections.

Download the Sparkfun library into your eagle lbr folder.
They have a component under M02, called M02PTH, that fits perfectly instead of the diode pads.
Will be less likely to rip the wires off the board that way.

U2 needs ground connected.
U1, U2, read their data sheet, might need to connect the enable pins to their Vin pins.
C6,C8, 10nF seems kinda small - I'd go with 100nF.
Select each component on the schematic, drag it up or down a little - make sure all pins are actually connected to the trace next to them.
Also run the Tools:Erc check, will help you find those too. U4 for example.

When done  moving parts, draw a polygon (Draw:Polygon) around the board, one each top & bottom, right-click each and Name them GND.  Will help with getting everything connected.

Man, 11:30 already. Will see what I can do with the other one.
Designing & building electrical circuits for over 25 years.  Screw Shield for Mega/Due/Uno,  Bobuino with ATMega1284P, & other '328P & '1284P creations & offerings at  my website.

xl97

WOW!..

thanks for the reply.. I guess I have more work to be done?  LOL

and I thought I was doing pretty good on the schematic portion at least!   lol

U2 is the new logic converter chip? (dont have it open currently?)

I added ground and name/value to it as well.. (thought I had uploaded that one as my last attempt?  perhaps not...)

I'll go over your point 1 by 1 tomorrow when I get into the office!

(gonna hit the sack now!)


thanks!


PS:
let me know if you have any questions on that change log!

CrossRoads

#21
May 23, 2012, 06:27 am Last Edit: May 23, 2012, 06:33 am by CrossRoads Reason: 1
"I guess I have more work to be done?"  Yes, a bit.
Schematic is nice, board layout needs revisting to make it work tho.

U1 & U2 are the voltage regulators.

The change log - what I wanted was a document that we could mark up & keep track of the design requirements, vs a never ending e-mail string where things get lost.
I currently have a 4-card design in the works, a 3-card design in the works, your update, another update that I ordered boards for over the weekend & need to order parts for, and another design that I am expecting details for shortly. So lets get semi-pro here on the requirements please.
Designing & building electrical circuits for over 25 years.  Screw Shield for Mega/Due/Uno,  Bobuino with ATMega1284P, & other '328P & '1284P creations & offerings at  my website.

xl97

thanks.. I'll make sure to focus on those vRegs tomorrow..



I thought I did provide a easy to follow, pointed list of design requirements/changes?

We dont need a new board..like the same footprint...etc.. but new DAC.. (same package but different pinout)  :smiley-red:

I'll try to organize it anyway you suggest!   :)

I wasnt aware you were still busy... I tried to check in every week or so... sorry.

thanks

CrossRoads

Thanks Jerry, I appreciate that.

I tried letting your design autoroute as it is while I was printing & saving stuff, I do that to get an idea of routability and see if placement needs work.
With the added ground planes (and before fixing up the areas noted) the router choked with 29 runs not connected, and those were going back forth across the board. Pretty sure you're going to need to update the placements to make that design fit.
One thing I do is number the decoupling caps for the pin they go next to on the uC, helps to visualize where they ought to be.
Designing & building electrical circuits for over 25 years.  Screw Shield for Mega/Due/Uno,  Bobuino with ATMega1284P, & other '328P & '1284P creations & offerings at  my website.

xl97

29  YIKES!


lol...


thanks for the tips.. Im on my way to the office soon (after kids get dropped off at school)..

and I'll go back over the the points you made.. (vRegs.. and numbering)..

the feedback is appreciated!   Im really starting to like Eagle more and more..  I just need some more experience/exposure..

maybe a smaller, goal/project?  something is smaller in size/requirements.. but still makes me utilize the basics in Eagle for?

well Im already into this project for a few hours.. so might as well stick it out!

thanks again..

CrossRoads

Or maybe a little larger footprint to start. Hard to cram a lot in a small space when the experience level is low. Gets better after a few boards.
Designing & building electrical circuits for over 25 years.  Screw Shield for Mega/Due/Uno,  Bobuino with ATMega1284P, & other '328P & '1284P creations & offerings at  my website.

xl97

good idea!  lol..

Im learning on the fly.. and taking things from other schematics and people 'approaches' to certian things!  lol

I copied the using a DIODE footprint for pads idea from you!  =)

a couple other things.. like having the I/O pads be a header set (5, 6,7..in a row..etc)

I was thinking.. is there a SINGLE 'through hole' like that that I can use?

I bet it would help for placement of the I/O-through holes if there they were singles.. instead of in set rows like that?

either way.. been swamped at work currently.. so I havent even opened up Eagle today!.. 



also.. question:

1.) when you hit auto route from Eagle.. will it do/add vias and traces to the bottom of the board for you? is that type of approach only done manually?


thanks

CrossRoads

Yes, you can find single holes and pads in the Sparkfun library if you have downloaded it.
The autoroute will connect top & bottom if it is able. Sometimes you have to help it out to finish. Like draw a trace as two segments, then right-click one of them and select properties, change the segment from one layer to the other, eagle will add the via for you. You may then want to select the via, change its shape, change its size.
I like iteadstudio for that, you can have 12mil via on 10mil trace, they can make it. Other places won't go that small.
Designing & building electrical circuits for over 25 years.  Screw Shield for Mega/Due/Uno,  Bobuino with ATMega1284P, & other '328P & '1284P creations & offerings at  my website.

xl97

awesome!  thanks.. thats what I was looking for!

and yes.. I LOVE the small traces and tiny vias you use and we got from iTead!!!!

I mean I like the footprint as it is now!.. no changes!  lol  hahaha


CrossRoads

Let the DAC/uSD board run last night, went to bed. 80% complete this morning. Have to look at how I jumbled stuff around, see what I can do so it can complete.
What are you planning for a cap? Needs to mount on pads due to uSD card underneath. Leaded part? Something surface mount?

Designing & building electrical circuits for over 25 years.  Screw Shield for Mega/Due/Uno,  Bobuino with ATMega1284P, & other '328P & '1284P creations & offerings at  my website.

Go Up