Go Down

Topic: Building a dual MCU project with two ATmega328 chips (Read 9 times) previous topic - next topic

pito

A high time to support the multicore arduino architectures with multicore programming IDE tools..
http://www.drdobbs.com/embedded-systems/multicore-programming-not-for-dummies/240148689
:P

Graynomad

#61
Apr 14, 2013, 01:51 am Last Edit: Apr 14, 2013, 03:55 am by Graynomad Reason: 1
@mihun70

Overall it looks pretty good and without more details and schematics it's hard to know exactly what does what, but I have the following comments

Is this single layer? If so you've done well.
What are the MOT headers for?
The headers don't appear to be aligned, for example DIG1 and PWM. While that has no effect electrically it's just bad form.
I don't see any good-sized power and ground traces. The ground traces I can identify are weedy little thing that run all over the board.
Most of the "ground plane" doesn't appear to be connected to anything.

EDIT:
The board doesn't need to be that large as there is a lot of blank space on the left and right sides. Is there a particular reason for that size?
There are no mounting holes.
As mentioned by us both I think the power rails are the biggest problem here, in fact I can't see where GND get to the chips unless it's through that component just above the "re" in "Core". That component appear to be a resistor which is unusual unless your measuring the current. Schematics would help.


______
Rob
Rob Gray aka the GRAYnomad www.robgray.com

Docedison

#62
Apr 14, 2013, 03:24 am Last Edit: Apr 14, 2013, 03:41 am by Docedison Reason: 1
Your Autorouter has a copper pour option called remove dead copper that would clean up your work considerably.. The only thing to watch for are islands of ground... or Vcc that have different net names which appears to be the case as Rob pointed out it is also a very good idea to check that the netlist and schematic drawing agree completely. This is a very  common mistake when combining different schematics via the copy paste option that most cad packages have. There is never too much time to make a board in because it would seem that there is always time to fix it.
When I designed circuit boards for a living I found the hard way.. on more than one occasion that checking the netlist against the schematic was a requirement that had some time to get my attention. When I did so I found that I made about 99% fewer errors with both the forgivable and forgettable and rarely ever made a bad board.. I've made my share of engineering errors and most of those repairable through part value changes because I do/did everything but thermal testing on bread boarded models of each module... This attention to detail generally is as close to true hindsight as one can get.
In the case of your PCB besides only presenting one layer shows clearly that the netlist wasn't justified against the schematic. Just print the netlist and schematic and cross off each net as you find it on the drawing by using a highlighter to trace the line on the schematic against the netlist entries and a very good idea to do the same with a checked out netlist against the PCB.
The PCB is Manufacturered from that netlist, If the netlist doesn't match the schematic properly one ends with a board that looks like yours.. The rather lengthy lines from controller to ground on the crystal pins are very long and totally un necessary... as well as being quite serious at higher frequencies their net names don't match those of the 'ground plane'.. I should think that "If" that board works it will not only be noisy but nave poor noise rejection as well again all due to the ground plane not doing the job it should ( No integrity of ground net names like gnd and GND and ground and Ground and Vss...
It makes no difference what you call it just make sure you call all of it the same. Remember that the ERC is about the electrical connectivity and all it takes is a ground symbol without a net name to turn your neat board into a real issue.

Bob
--> WA7EMS <--
"The solution of every problem is another problem." -Johann Wolfgang von Goethe
I do answer technical questions PM'd to me with whatever is in my clipboard

mihun70

#63
Apr 14, 2013, 08:25 am Last Edit: Apr 14, 2013, 08:43 am by mihun70 Reason: 1

@mihun70

Overall it looks pretty good and without more details and schematics it's hard to know exactly what does what, but I have the following comments

Is this single layer? If so you've done well.
What are the MOT headers for?
The headers don't appear to be aligned, for example DIG1 and PWM. While that has no effect electrically it's just bad form.
I don't see any good-sized power and ground traces. The ground traces I can identify are weedy little thing that run all over the board.
Most of the "ground plane" doesn't appear to be connected to anything.

EDIT:
The board doesn't need to be that large as there is a lot of blank space on the left and right sides. Is there a particular reason for that size?
There are no mounting holes.
As mentioned by us both I think the power rails are the biggest problem here, in fact I can't see where GND get to the chips unless it's through that component just above the "re" in "Core". That component appear to be a resistor which is unusual unless your measuring the current. Schematics would help.

______
Rob

Yes! the board must be fixed on a part of my project and the left and right space is for mounting holes;
The Mot are for 2 brushless motors..
Parts of gnd are not to consume too much chloride or cutter fairy on CNC.Depends if oane  teacher will help me with  CNC.
this is a beta form.Are next the mounting holes i need to take one calliper from my friends...i don't have one for me...and i see that is needet the vcc trace to be bigger...
i worked with the 0.45 and 0.6 mm
the board is single layer 120 x70 mm
i'm not an expert I got acquainted with Altium a month ago..On my university until now(i'm on 2-nd year)i don't have learn any pcb stuf...
The netlist is checked...and will be rechecked...the nets are carefully chosen and used...
if someoane is interesed...i cand put the schmatics here...


Graynomad

#64
Apr 14, 2013, 10:35 am Last Edit: Apr 14, 2013, 10:37 am by Graynomad Reason: 1
Quote
The Mot are for 2 brushless motors..

Then I hope they are really small ones, those traces are very narrow.

Quote
Parts of gnd are not to consume too much chloride or cutter fairy on CNC

OK, that's common when hand making boards.

Yes please post the schematic, it will allow us to more properly identify issues.

In Altium the netlist checking is part of the process, no need to print and "greenline" as we used to do.

For that matter I use Altium, if you post the PcbDoc file I can review it properly.

______
Rob
Rob Gray aka the GRAYnomad www.robgray.com

mihun70

#65
Apr 14, 2013, 10:53 am Last Edit: Apr 14, 2013, 11:38 am by mihun70 Reason: 1
The motors have separatly power supply.The vcc from there can not to be used!is only for driver supply!RS-s are just 0 ohm rezistors to get over trails..the p1 and 2 are for icsp...will be used one time to burn bootloader..

Graynomad

Got the Altium design files.

First thing I noticed is that these pins are not connected to GND



Note I changed the colour to blue, red was too hard on my tired eyes :)

Next thing, there are no decoupling caps near the CPUs, I assume that's what C3, 4, 5 and 6 are supposed to be but they are MILES away from the power pins on the chips.

That's all for now, but those power traces really need beefing up. I'll look at them next.

______
Rob
Rob Gray aka the GRAYnomad www.robgray.com

Graynomad

You have screen printing all over the place, some even over component pads



______
Rob
Rob Gray aka the GRAYnomad www.robgray.com

mihun70

The gnd bug i have "fixet" after i sent you the files.. before to make modifications to the board i remove the power plane...and put again ...it took me days to configure this board and i don't want to start over...i don't have place neear the cpus.I have carry out to be at least one cap near each cpu.i know the 3d pads are not ok...but when i print the pdf  i have all pads.

Graynomad

Quote
before to make modifications to the board i remove the power plane...and put again

If you just want to get it out of the way it's easier to "shelve" the plane

Tools>Polygon Pours>Shelve X polygon(s)

Quote
i don't have place neear the cpus.

Here's one done, it took 20 seconds, Ok maybe a minute.



______
Rob
Rob Gray aka the GRAYnomad www.robgray.com

mihun70


Quote

Here's one done, it took 20 seconds, Ok maybe a minute.



Good place! i see that you have altium skils...can you help me with 4 holes?I tryed to put  them with the mouse  but never milimetricaly...  i don't know an option like in autocad...if you help me with this...please 10 mm from left and from right and 8.5 mm from up and from down(don't know to tell right in english :smiley-roll-blue:)

Graynomad

Double click on the component (in this case the hole) and type in the X and Y values. The values are relative to the origin, either place that in one corner and do the maths or move it around the corners and enter

10,8.5
-10,8.5
10,-8.5
-10,-8.5

respectively for each hole.

You move the origin with

Edit>Origin>Set

If you are in imperial measurement mode type "Q" to swap to metric.

______
Rob
Rob Gray aka the GRAYnomad www.robgray.com

mihun70

i think that i have setted ok...but not
10,8.5
-10,8.5
10,-8.5
-10,-8.5


10,8.5/110,8.5/110,61.5/10,61.5

can you send me back files after you modificated  them?with those cap ?
or is my job to redo the work? :smiley-roll-sweat:

Graynomad

Quote
10,8.5/110,8.5/110,61.5/10,61.5

Like I said, "either place that in one corner and do the maths or move it around the corners and enter..."

You chose the first option.

Quote
or is my job to redo the work?

Yep, you should be able to do that faster than I could ZIP and email the files. :) There's so much room around those chips you could drive a bus through there.

Anyway I did not save the changes, plus I deleted all the logos because they made it too slow to re-pour the plane. 

While your at it increase the size of every power trace where you can. Make them as large as possible.

______
Rob
Rob Gray aka the GRAYnomad www.robgray.com

mihun70

I have now 2 caps near each IC... :smiley-sad-blue: thx for modificated files =( (romanian humor)

Go Up