Soldering and first pcb with Eagle

Developing my very first pcb in Eagle:

See attached picture.

I placed some components on the bottom but see red and blue going to different pins of that bottom part? Can I solder this bottom component on either side? Or do I have to solder both sides, or just the side where the route leads to. (red=solder bottom, blue= solder top)

The arduino mini pro VCC pins are connected by eagle, does(n't) that matter?

Left pads (octagon) are taken from a header file and right round pins are for a lcd. Inside octagon showing a square layer (51tDocu). Are those just different size pads but handled the same way as the round pads, or why would someone use octagon shaped pads?

red is top-side, blue is bottom. If you have all through-hole components then it doesn't matter which side the traces run. The software assumes double sided board with plated- through holes. If you are only designing for single sided board + through-hole components you should use only blue traces.

You should edit the power/GND traces to be thicker (40 or 50 thou), and maybe learn about groundplanes and polygons.

If you're getting the boards made up by a board house then the holes will be plated i.e. there'll be a thin layer of conducting material plated around the inside of the hole so the top and bottom pads will be connected so you'll only need to solder the bottom pads.

If you're making up the board yourself then they won't be plated.

You should note that Eagle will assume that the holes are plated for both auto-routing and DRC checks.

Oke, got it. Components on top, blue traces on the bottom and vice versa. Meaning the green pads shown are on both sides so I can solder regardless the color of the trace ?

(I thought the pads would only be visible according the color of the trace it's connected to...)

You should edit the power/GND traces to be thicker (40 or 50 thou), and maybe learn about groundplanes and polygons.

@MarkT: thx for the tip, will do!! Thanks for noticing cause didn't consider or hear about it ..yet...

If you're getting the boards made up by a board house then...

@GilchristT : yes, by a board house 2 layered board. I'll need to check to make sure they also produce plated- through holes.

Eagle will assume that the holes are plated for both auto-routing and DRC checks.

@GilchristT: oke!

so you'll only need to solder the bottom pads.

@GilchristT: ? only bottom pads? I have components on both sides, so I'll probably need to solder on both sides . That'll be no problem as I now assume the (green colored) pads are on both sides and connected by plated-through holes.

creamers: @GilchristT: ? only bottom pads? I have components on both sides, so I'll need to solder (where possible) on both sides. That'll be no problem as I now assume the (green colored) pads are on both sides and connected by plated-through holes.

So long as the holes are plated (definitely do check with your board house to be sure to be sure but it's fairly standard) then you only need to apply solder on one side for each through-hole component. It can be either side depending on what's easiest for you but you don't need to solder both sides.

What can be useful to get an idea of what your board will look like is to create Gerber files. This used to scare me but, like everything else, it's simple once you know how. Then use a Gerber Viewer, there are a few available free online, to look at each layer of the board and how they stack up.

@GilchristT: Thx!!

Now I need to find out more about power/GND traces, groundplanes and polygons in combination with Eagle and see when or if it's needed for my board.

You should edit the power/GND traces to be thicker (40 or 50 thou), and maybe learn about groundplanes and polygons.

I practiced some more with Eagle and readup on polygon's , orphans, thermals etc.

But, is it alright to put a complete polygon over the 2 layered board (or at least a big polygon), one vcc (top) and one (bottom) gnd polygon. Isolate value a little bigger to give the other pins enough room. The jackplug, 2xIRF540 , screwterminals and the 7808 are close to each other so the big polygon can handle the 12v28amps.

What are the (dis)advantages of doing this? Is it still safe doing this or should I consider lowering my max amps (18amps)

(btw, I also adjusted my schematic and added two fuses:)

Two layers, two polygons:

Just a 12mm width polygon/trace:

Please advice ;)

It is not typical to have one side the Vcc plane and the other Gnd. Usually a Polygon is drawn over both layers, Name them GND, then let the autorouter connect all the GND pins to it. May need to add some vias, Name them GND, to connect the top & bottom planes together.

Edit:Net classes, make the default trace something like 10 mil wide, 10 mil clearance, 12 mil drill. Add one called Power, 24 mil wide, 10 mil clearance, 24 mil drill. You can also make traces wider manually as you did in reply #6.

I see your barrel jack is not connected to anything yet.

Check the ratings on your components - 18A is lot for a barrel jack or a screw terminal. Also check google for a "trace width calculator" website like this one to see how wide a trace you need to support 18A. http://www.multek.se/engelska/engineering/pcb-structures-2/trace-width-calculator The thickness of the copper (1 oz or 2oz/sq ft) is important, as well as being an external trace (2-sided boards have the copper on external layers, while 4-layer boards will 2 external and 2 internal layers).

A 4-layer board often has a power plane but a 2-layer should have polygons for ground only, on both sides. Have a look at the excellent boards done by Sparfun or Adafruit. They publish their Eagle files online and you can learn a lot from them.

For 'high power' traces between the big MOSFET and the input/output terminals, I usually use fat traces in Eagle, although a polygon might be useful for some routing. Another trick to get really high current is to draw 'wires' in the solder mask layer over the top of them (areas which will have no mask) and then run a bead of solder along the traces.

Don't increase the clearance, you want the ground planes to squeeze between other pins and reach all areas of the board.

Turn on the "Thermals" option. It will make it much easier to solder the components which have connections to the ground plane.

Great tips!!

Another trick to get really high current is to draw 'wires' in the solder mask layer over the top of them (areas which will have no mask) and then run a bead of solder along the traces.,

@MorganS: thanks for the tip to search for eagle examples at sparkfun etc. Any change you got an Eagle example of your own ?

Thermals on - easier to solder, that's logical when using a gnd polygon on both sides. But I assume that a fat 'trace' made by a polygon should not have thermals so it can dissipate heat better.

Will take my time to investigate, read and learn some more considering those tips. Thx.!

creamers: @MorganS: thanks for the tip to search for eagle examples at sparkfun etc. Any change you got an Eagle example of your own ?

Just draw wires or rectangles in the tStop or bStop (for top or bottom) layers over the existing traces and you'll then see the diagonal hatching that is identical to the hatching on other solderable pads. Definitely a good idea to verify everything using a gerber viewer.

If you draw areas of traces, Name them the signal name you are connecting to. Same for adding Wires - Name them. If you make blocks using Rectangles, you can't Name them.

'high power' traces between the big MOSFET and the input/output terminals

Just draw wires or rectangles in the tStop or bStop (for top or bottom) layers over the existing traces

Fat traces with bStop wire layer, see pictures.

Net classes, make the default trace something like 10 mil wide, 10 mil clearance, 12 mil drill. Add one called Power, 24 mil wide, 10 mil clearance, 24 mil drill.

Added one called Power and connected them to the 'high power' schematic wires. But made the traces bigger.

Name them GND, to connect the bottom and top planes together.

placed the groundplanes on top & bottom .

May need to add some vias

I didn't do this, but while writing it remembers me. I don't see them created by the autorout function.

Don't increase the clearance, you want the ground planes to squeeze between other pins and reach all areas of the board.

Didnt adjust the settings, so spacing is 0.05 and isolate is 0. Good enough?

Any comments / advice ? Thanks for helping!

creamers: @MorganS: thanks for the tip to search for eagle examples at sparkfun etc. Any change you got an Eagle example of your own ?

Thermals on - easier to solder, that's logical when using a gnd polygon on both sides. But I assume that a fat 'trace' made by a polygon should not have thermals so it can dissipate heat better.

No, I don't have any of my own Eagle files online anywhere.

It looks like you want a high-current trace. Putting a thermal relief on that trace doesn't make much difference, because it's only a fraction of a milimeter long. Yes, that fraction will heat up a bit but it's attached to a heavy trace which will dissipate heat. If you have a good temperature-controlled iron, then it's not so difficult to solder without the thermals. For high-current traces, I will sometimes do them without thermals. For general ground plane stuff, I always use the thermals option.

Any others who can comment on my eagle pcb ?

Let's top & bottom seperately with their ground planes.

Not easy to see at that size but...

Is there a ground plane? Doesn't look like it because it seems to have tracks connecting the ground pins I can identify.

What is the fuse on the left supposed to do? Does this have high current through it or is it just protecting the Arduino? What happens when the fuse blows - can the high voltage on the input side feed into the Arduino's inputs when the fuse is out? This can be a serious problem as the input voltage limit for the pins isn't just "5v" but it also isn't allowed to be higher than the Vcc. 5V on an input and 0v on Vcc will toast the chip.

I wold suggest putting the fuses together on the right side - make a kind of firewall between the unprotected inputs and the rest of the circuit. This is especially important if it's possible to get mains voltage on the inputs via any kind of screwup.

You have fat high-current tracks going to one pin on each output connector. What about the return current or does that go off-board to a remote grounding point?

It looks like you used the auto-router. Can you see what it did there? All the top tracks are 90 degrees to the bottom tracks. If you are laying it out manually, try to follow this 90 degree idea - make all the blue tracks vertical and the red tracks horizontal.

Not easy to see at that size but...

if you click on it, it'll be better to see

Is there a ground plane? Doesn't look like it because it seems to have tracks connecting the ground pins I can identify.

You were right, somehow I thought it was right. Found also a good trick to see if the gnd traces go into the groundplane by using: run length (it shows zero length for gnd, so they go all into the groundplanes I assume)

hat is the fuse on the left supposed to do? Does this have high current through it or is it just protecting the Arduino?

it's adviced in this thread to use two fuses. And this fuse on the left is getting 8v from the 7808 into the raw arduino input.

I wold suggest putting the fuses together on the right side - make a kind of firewall between the unprotected inputs and the rest of the circuit.

Don't understand what you mean by firewall between the unprotected inputs. 12v in - fuse - 7808 - fuse - arduino raw in.

You have fat high-current tracks going to one pin on each output connector. What about the return current or does that go off-board to a remote grounding point?

12v to feed ledstrips on each output connector. Using irf540 to pwm ledstrip on gnd output pins.

It looks like you used the auto-router. Can you see what it did there? All the top tracks are 90 degrees to the bottom tracks. If you are laying it out manually, try to follow this 90 degree idea - make all the blue tracks vertical and the red tracks horizontal.

Wouldn't this create alot of VIA's ?

Vias are not expensive. The board looks neater with fewer vias but unless your manufacturing costs 1 cent per via, I wouldn't care about how many there.

Can the 7808 pass enough current to pop the fuse? (Without popping the 7808?) What happens to the 7808 after the fuse blows?

The firewall idea is just in case some idiot (ie. you with a momentary brain-fade) plugs the board into 220V and you want the fuse to blow to protect your circuit. If the traces going to the fuse are very close to the 'delicate' pins of your Arduino, the voltage can jump to those pins and blow your circuit anyway. Think of a momentary surge of 100A and this will look for somewhere to go when the fuse goes. Induction will give very high voltage spikes - much higher than your input voltage.

So everything that's 'unprotected' on one side of the fuse should be on one side of the board with a gap between those traces and every other trace or pin.

One interesting board I found once was for a weather station, which had wires running up to the anemometer on the roof. This had a lot of lighting protection on it. The lightning protection wouldn't save the board but it would stop it bursting into flame and burning down my house.

Thnks for explaining. Just ran auto route again, but for practice I should try to do it manually.

PCB

I really don't have enough knowledge about electronics to know that much or forsee that much, I just hope you guys get me to work...;)

(I had a second screw term input but replaced it with a jackslt. My assumtion is that using (twice) 12v adapter is safer than using a screw term as input. Also, if it blows, than I don't care about the arduino pro mini. Total cost are not that big. But,.....I do care about my house....! :)