Go Down

Topic: ATMEL Mega1284P evaluation board avalible (Read 178412 times) previous topic - next topic

skyjumper

Crossroads, keep in mind that the board we did also failed many of those checks but there was no problem making the PCBs.

CrossRoads

Yes, but:  the initial design could not autoroute. I then did a manual route and solved many of the issues by moving components, and ended with ugly looking traces at funny angles & stuff (routing with laptop finger pad is not the best way to go). I was able to get that to autoroute with a couple more small moves and only had to manual fix up 3-4 traces, so the traces ended more or less like my manual version but much neater looking. Eagle maintained the clearances and selected the drill sizes & stuff so the errors were limited to tStop & tCream overlaps, which some sliding & scooching around resolved.

The same approach is not working so well here with the FTDI chip, the SD card driver, the RS232 driver, all of which the other also had, but also the RTC, smaller board size, jumper fields for user signal manipulations, etc. I had the manual routing done, looks like a checkerboard pattern, but it won't autoroute. Also want to incorporate your suggestion on the square pads vs round.

I haven't looked at the international circuits Design Rules yet, not sure where that will lead.

Solution might be to widen/lengthen the board, have the atmega placed closer to the digital header pins and move the  support chips to the 'analog' side of the DIP.

I still think the original shield pin assignments are part of the problem, with signals criss-crossing the board.
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.

skyjumper

Maybe its time to drop Eagle and go to a 4 layer board!  LOL

Actually my friend Bill was over the other day and showed me the GNU EDA suite. All free, very nice stuff with schematic capture, board layout, auto-routing, component libraries (he should me how to add a component - not too hard).  No limit on board size and works up to 8 layers. He said the only restriction of consequence is that all the vias have to go all the way through the board.

Non-triveal to learn though, like all these things. :-( Who has time to invest in learning a new system?

Is there a reason you didn;t want to make the Bobuino board any bigger?



CrossRoads

Size: I started out just planning to use the SMD 1284, plenty of room for the RS232, SD driver & socket, 1 more header for the extra I/O, no big deal, and it fit nice in the lengthened Uno footprint (lengthened for the SD socket and the DB9 when I had that in the design).
So when I went to the DIP, figured it would still fit as the # of signals hadn't changed. But now its feeling really condensed.
Still, I am very close, I want to get it done now. My newness to the tool is getting in the way despite being able to do more with it, or at least do it quicker, every time I use it.
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.

48X24X48X

Cross,

If you don't mind posting the Eagle files, I think everyone here can take a look and help or suggest.
I'm not a pro in Eagle, but I'm familiar with a number of CAD. And I think there's a lot of Eagle master here to help out!

If you do move the chip upward, you might have more signal issues later especially on the analog lines. I faced this before and I end up getting kHz noise on analog lines.

IMHO think the board is still achievable with 2 layer! And it doesn't matter what CAD you use, as long you stick to one that you like or prefer, it's good enough.

CrossRoads

The board file can be downloaded here.
I don't have access to this stuff during the day, end up getting to play after fencing classes at night.
http://www.crossroadsfencing.com/atmega1284_Rev7_auto_routing.brd
http://www.crossroadsfencing.com/Fusion_eagle_rule_v1.1.dru
(right click, save target as, ... etc and correct the file extension).
I already cleared up the Clearance errors. Except for the built in error in the SD card socket.
The Drill Size and Width errors are the ones I am concerned about.
The Stop Mask errors are just the part outlines on the header pads, seems like a stupid error to be getting.
The Default setting creates tons! of errors.
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.

48X24X48X

Some thoughts on the boards:

  • All 2.54mm connectors, you might want to align them to 0.1" grid. People might want to stack some cheap perf board on top. You can do this in Eagle by relying on the grid setting of 0.1".

  • Your irregular angles of traces is splitting a lot of ground pours. One good example, A6 & A7 traces underneath the ATMEGA1284P on the bottom layer. If these 2 traces follow 45 degree and bends only after moving slightly to right, your ground pour will be able to cover the bottom of the IC.

  • Part placement location. I tend to place components that has shared lines nearer to each other to reduce the number of traces going to 2 different locations. An example, the RTC usage of the SDA & SCL pins. Yes, on 1st thoughts your RTC is nearer to the PC0 & PC1. But at the same time your breakout header is located on the other side of the board. If you can place the RTC nearer to breakout header, you'll save some routing traces. Don't worry about the length of I2C lines, 3 cm is not much!

  • Guard rings for crystal. You might want to have ground surrounding the crystals and pilled some small vias to the ground on the bottom layer. Avoid having other lines going underneath the crystal. Maxim datasheet have plenty of example on this.



If there's plan to stick to microSD connector only, there's plenty that you can do to improve. For example, you can push the microSD to the left top nearer to SPI breakout. By doing that, your RTC and battery can move to the right edge of the board (original location of SD) and you can even replace the battery connector with a slide in version from the edge of the board like this one: http://www.sparkfun.com/products/8863

That's some of my humble thoughts. What the rest of you guys think?

skyjumper

Okay, I am going to stop my serial read-write process. Its been running non-stop since I started it.

However, this does not prove much. Maybe Atmel fixed the bug, but there are some chips out that still have it. Maybe I just didn't write code to trigger it. The high pass filter may be a good idea, just in case.

48X24X48X


Okay, I am going to stop my serial read-write process. Its been running non-stop since I started it.

However, this does not prove much. Maybe Atmel fixed the bug, but there are some chips out that still have it. Maybe I just didn't write code to trigger it. The high pass filter may be a good idea, just in case.



The errata is empty in the datasheet. I never see any chip that is perfect!

CrossRoads

Okay, I have the ground planes covering just about everything except a few small areas where there too many line in parallel to get any coverage. I'v got the signals moved away from the crystals and ground plane underneath them on both layers (altho my wirewrap boards have just ungrounded copper holes underneath and wires there too and it doesn't seem to bother anything as evidenced by skymaster's testing of the "hacking the Uno" prototype.
I was looking at the runs last night, and it looks like I managed to put vias in the middle of 2 IC pads, so I have a little more cleanup to do. I think I have all the clearance between traces & pads cleaned up.  Got most of the Width errors cleaned up, they mostly seemed to 10 mil traces for power & ground, so have been making them wider, like the 16 mil that is the defaut in eagle.
Don't know why, but the drill size errors seem to have gone away on their own.
And , need to clean up the silkscreen/labelling so parts placement is readable. Possibly move the headers for the extra IO and RS232 IO to conform to same 0.1" grid alignment as the shields. (maybe add 2nd set of holes so the funny offset shiedld can be populated for a standard shield, or for normally spaced perfboard - need to see if any traces are in the way). The others are intended to have jumpers installed for signal selection.

Have not tried updating the SD socket symblo yet (still keeping both) or changing 0805 pads to squares from round. I think for that I have to delete them on the schematic, add them in again, and then see if they will fit in the same space on the board.
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.

tastewar


... or changing 0805 pads to squares from round. I think for that I have to delete them on the schematic, add them in again, and then see if they will fit in the same space on the board.


Sheesh. I'd have hoped/thought that the pads would just be a property of the component that could be changed easily. Of course I've never used Eagle (or any other) CAD software...

skyjumper

And , need to clean up the silkscreen/labelling so parts placement is readable.


The default silk screen line width is too narrow and it will fail DRM at Advanced Circuits and one other (I forget who). But on the plus side, they correct this for you. International Circuits never said a word about it and it came out great. I did make a change to the font I think to proportional. I'll double check and post back.

Quote
Have not tried updating the SD socket symblo yet (still keeping both) or changing 0805 pads to squares from round. I think for that I have to delete them on the schematic, add them in again, and then see if they will fit in the same space on the board.


On the pads, thats super easy. Right click ont eh component, and I think under properties just change the packahe type from 0805RND to 0805. If you want to round the corners, this is set in the Shapes tab of the DRC menu. It's not necessary to create new footprints.


skyjumper

Sheesh. I'd have hoped/thought that the pads would just be a property of the component that could be changed easily. Of course I've never used Eagle (or any other) CAD software...


I *think* the way this works is that each compnent has a "package" property and it just needs to be changed.

I'm also not certain that its better to use square. There dos not seem to be a concensus on this. I plan to reflow some boards between now and Sunday and the boards have round pads for 0805 components. We'll see how it works.

mowcius

Quote
Have not tried updating the SD socket symblo yet (still keeping both) or changing 0805 pads to squares from round. I think for that I have to delete them on the schematic, add them in again, and then see if they will fit in the same space on the board.

Assuming the parts have the same number of connections in the same order then you can just use the 'Replace part' tool which seems to work pretty well when people have the wrong package for a chip or similar.

CrossRoads

The SD socket for the FCI part I want to use does not exist that I know - or if it does, I haven't found it (am still fighting my way along with eagle). I will admit to stumbling along in my library searches.

digikey catalog
http://search.digikey.com/scripts/DkSearch/dksus.dll?Detail&name=609-3956-1-ND
datasheet
http://portal.fciconnect.com/res/en/pdffiles/doc_search/10067847.pdf
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