Hi,
this is the first time i want to use a pcb service. So this is my first time creating a board.
Can you tell me if it will work or if I have any mistakes?
The mosfets are IRLML2502.
Resistors will be about 180 Ohms.
Is that DC Jack connector correctly attached? And im not sure about those big drillholes. But I found this jack in a library.
Its a shield for mega to control LED stripes.
Is X2 or the DC jack going to "run into" the USB connector or DC jack on the Arduino below?
Btw, nice use of the ground planes! Most people miss that on their first board.
Wires in schematics usually only run at 90 degree angles, the connection from R1 to the connector pin is touching the ground wire, not going to cause problems, but its not very neat.
In the PCB, those vias that are placed around the ground plane are not actually connected to anything, I'm guessing they're meant to be connecting the top and bottom planes together?
Did you NAME your Polygons and the Vias GND?
Hi,
thx for your replies.
Is X2 or the DC jack going to "run into" the USB connector or DC jack on the Arduino below?
nothing of both is running into the arduino. Only the header connectors. I thought its better to completly leave the arduino out of the 12V opposing to plug the jack into arduino and grab the 12V from vin, isnt that correct?
not going to cause problems, but its not very neat
thx i fixed that
In the PCB, those vias that are placed around the ground plane are not actually connected to anything, I'm guessing they're meant to be connecting the top and bottom planes together?
Did you NAME your Polygons and the Vias GND?
thx, forgot to name the vias gnd
Anything else as suggestions?
Im still not certain with that dc connector, even in the schematic it looks odd.
lax123:
Is X2 or the DC jack going to "run into" the USB connector or DC jack on the Arduino below?
nothing of both is running into the arduino. Only the header connectors. I thought its better to completly leave the arduino out of the 12V opposing to plug the jack into arduino and grab the 12V from vin, isnt that correct?
No I mean physically run into. Both the USB connector and the DC Jack on the Arduino boards are relatively tall (sometimes taller than most header pins.) I would make sure that, physically, the header pins X2 aren't in the same area as the Arduino's USB connector. That's usually a problem for most shields.
While, Barrel Jacks tend to have relatively large leads which stick out a little farther on the bottom which might interfere with the barrel jack below it.
lax123:
Im still not certain with that dc connector, even in the schematic it looks odd.
What looks odd?
No I mean physically run into.
Ah good point, i didnt think about that but im lucky, my shield is only about 5mm larger then the arduino top pinrow.
Looking at the arduino dc jack pins it seem that there should be enough space between the capacitors of ardu and the jack on the shield as the pin connectors between ardu and shield will also give some additional height.
the meaning of the dc jack schematics symbol is not obvious to me.
lax123:
the meaning of the dc jack schematics symbol is not obvious to me.
Because there are two "ground" connections? One is disconnected when there isn't anything inserted into the jack. Most people just connect both, like you did.
well not so important. its not about the 2 gnd, its just that symbol for the jack in the schematic isnt self explanatory, atleast for me.
I have another issue, maybe someone knows an answer.
The via-headers in the brd are actually vias i made in to a library part with pins so that i can actually attach something to these vias in the schematic.
The seeedstudio DRC tells me "dimensions error" on all of these via-headers.
So i guess the part is too close to the edge, but on the other hand when i just place a simple via with the same size and same distance to the boards edge i dont get an error. I guess drc thinks my via header is a "part" so it must not be that close, but if it was just a via (so just as it is) its ok.
Do you have an idea whats wrong?
In my attachment I put a simple via left of my via-header, as you can see it doesnt get marked red
Can you post a screenshot with the DRC error window and highlight on PCB.
Or post PCB file with the DRU file you're using.
X3 pin 4 has a "less than 90 degrees angle"
that will make what's called an acid-trap
means the track will over etch in the corner
try to avoid < 90 angles
I always go for 45 degrees everywhere
that'll be 2p 2c depending on location 
I think your pads are too close to the edge. DRC didn't like it.
Need a resistor between gate and ground for the mosfets.
Why not use pads instead of vias to connect your wires?
and just because a PCB fab can do 6/6mils doesn't mean you have to in your boards.
Personally, I like a bit more trace clearances if there is enough room to do it anyway.
Name your vias GND so it connects both top and bottom copper layers. Right now, your scattered vias aren't doing anything.
X3 pin 4 has a "less than 90 degrees angle"
I made a T out of it.
Name your vias GND so it connects both top and bottom copper layers
I already fixed that, see last my attachment picture.
Why not use pads instead of vias to connect your wires?
Could you explain more please as I am unexperienced. I use the vias for their holes to put headers in them so that i can attach my shield on top of arduino.
I think your pads are too close to the edge. DRC didn't like it.
Why doesnt drc like my library part consisting of vias, but likes plain vias at the same position with the same size? I could just place a Via same size same distance next to my existing header-vias and it would give me no error.
I use the vias for their holes to put headers in them so that i can attach my shield on top of arduino.
Why not use a header part library. There's plenty in Eagle.
(though electrically, either one will work... but it's best to get into the habit of using the correct part library for it's purpose.)
Why doesnt drc like my library part consisting of vias, but likes plain vias at the same position with the same size? I could just place a Via same size same distance next to my existing header-vias and it would give me no error.
In DRC, there's several "rules" and clearances. Different clearance values for pads, vias, traces, edges, etc... It may be the clearance numbers for the vias was just enough to pass.
Vias are usually used for connecting top and bottom traces together. (say you need to move signal/voltage from top to bottom, you use a via)
Also used to tie the top copper pour with the bottom copper for ground planes, or heatsinking purposes.
Vias are not used as a convenient hole to connect or solder parts/wires/headers into them.
Use wire pads, or header parts for this purpose.
So I just could ignore those errors as its not actually a part but several vias combined?
Well actually I used "real" connectors at first but they didnt work as they are like 2 mm too large and wont fit on the 5x5cm (see attachment)
Otherwise I would not have gone through the trouble of creating a new part for the library, creating footp and symbol and pinconnections. But maybe there is a more clever way I dont know of.
You can change your pads from oval to a round, or square.
If you have the actual part you'll be using, measure it with a digital caliper and see if it will really fit or not. Sometimes, the part outlines in these libraries are not accurate (too small or too large).
Now, whether you can ignore these DRC issues or not, well... it's up to you.
This is just a computer screen.
You can make it "work" on your computer screen, but who knows... you may be surprised when you get your boards back from the PCB fab house and it's not what you expected.
or it "works" on your computer screen but the PCB fab house wouldn't manufacture it because it didn't conform to their DRC.
There are certain DRC warnings I ignore, but only because I know my PCB fab house and know they can manufacture it without problems.
Seeed will allow the pads that close to the edge. The extreme would be castellated pads and that is possible with their service.
Not really a good practice though. You've got lots of board space and you should use it rather than creating physically weak areas on the edge of your board.
You've got lots of board space and you should use it rather than creating physically weak areas on the edge of your board
how can i achieve that? mega is 5,5cm wide and seeed max 5 cm (unless i want to pay extra 15$ for 5mm), so these connectors have to be that close to the edge otherwise it wont fit on the mega
Whoops I was totally oblivious to the fact that this is a shield.
Here's an example of a Seeed user that created a shield using their service and squeezed their pin holes right on the edge like you're doing. Worked for him so you should be OK.
