EAGLE dimensions/drill issue

We can’t see the names of the wires in that image. I guess VCC is the red (top layer) trace. That looks like it makes an adequate connection with the pads. It should normally snap to the center of the pad. Did you route it with the Line command or the Route command? They’re right next to each other and both put copper on the board but Route is the correct one for replacing airwires with real wires.

The blue trace (ground?) is more worrying. It is on the other layer so while it crosses the connector, it doesn’t connect to it.

When you are routing with the Route command, you can switch layers at any point. It will automatically place a via for you, with the current Via settings. If you start a trace from any pad, it will switch layers to start with the pad’s layer.

Ok Im trying to use the Ground Plane to help me with the routing. Here is what I started out with:

Screen Shot 2017-09-02 at 7.16.46 AM.png

then I chose these options:

and would get this:

Screen Shot 2017-09-02 at 7.18.59 AM.png

which isnt right so I unrouted the ground traces I had, then hit Ratsnest again and finally got this:

which seems right. I can see the top flex connector, middle piezo, bottom IC, power connector and ISP GND connections connecting to the ground plane. But there are 2 problems:

  1. The GND between the capacitor, ISP and power connector are not connected to GND for some reason.

  2. I still have crossing/overlapping traces from the ISP to the IC

Screen Shot 2017-09-02 at 7.16.46 AM.png

Screen Shot 2017-09-02 at 7.18.59 AM.png

Oh cool, I was able to route the cap+ up to the resistor. I think it hadnt made the connection because it crossed the other pad of the cap(-) which would have made a short. So I routed it around the cap.

Now it connected the cap pad to GND and the ISP GND to the ground plane as it should but I still have a rastnest wire from cap GND to ISP GND for some reason...

And the overlapping traces which I need to solve for.

Ok I re-routed a trace and I have only these overlaps left:

I could either move the one-highlighted trace from ISP-IC-R to the back of the board (bottom blue layer),
or I could leave this one on top and move the other two-unhighlighted-overlapped traces to the back. What do you suggest?

First move the decoupling capacitor right next to the supply pin on the chip. Which trace you choose
to route underneath is pretty arbitrary. If your groundplane is top-side most signals should be
routed on the bottom side of the board, otherwise they break up the groundplane.

The trace between IC and ISP connector could travel through the ISP connector.
The trace going up could go between the IC pins (three traces there).
The horizontal part of the trace above the word TINY could go up a bit, so the flood-fill will reach the ground pin of the ISP connector.

Reduce "isolate" and "width" on the ground plane to the minimums specified by your manufacturer. Then it will squeeze between the pins better.

Yeay! Im getting there:

About the width and isolate, I made isolate on the ground plane 0.024. Width is set to 0.016. So as far as ive read, " Isolate setting which defines how much clearance the ground pour gives other signals". That means how much space it leaves between other signal traces and the ground plane?

I assume "width" is the thickness of the traces? What is a good number? As I mentioned, 0.016 is default in my case.


My preferred PCB manufacturer, OSHPark, can draw traces as narrow as 6mil, with 6mil spaces between them. That would be 0.006

I don't normally make traces smaller than 10mil but I do allow ground planes to use the 6mil minimum.

Isolate can be set to 0 as the design rules will enforce the 6mil clearance, as well as the clearance to the board edges. (called "dimension") Isolate is only relevant for planes that border other planes.

Depending on what you're screwing into the mounting holes, you may want to keep the ground plane further away from the edges of the holes. You can add a circle on the tRestrict layer to stop the ground plane going too close to the holes or just turn up the dimension clearance to do it everywhere.

You did download or transcribe the design rules from your manufacturer, didn't you?

Depending on what you're screwing into the mounting holes, you may want to keep the ground plane further away from the edges of the holes.

I think a 3mm (or 3.2mm) hole from the 'holes' library takes care of all of that.
A cheese-head screw will stay inside the outer circle.

That layout is looking much neater now.

Signal traces are thin, 10 to 16 mil, power traces thick, 32 to 50 mil. The thicker
traces for power are thicker so they have low inductance, since the resistance is already low enough
for logic chips (assuming the current draw isn't very large).

Inductance matters for fast switching chips like logic chips where the supply current varies on
nano-second timescales and you don't want the supply voltage at the chip to vary by more than
a few 100mV. This is why the decoupling capacitor needs to be close and connected with wide traces.

However you still have breaks in the ground-plane continuity - it needs to approximate an unbroken
sheet. This is why I've suggested having it on the opposite side of the board to all the signals.

Have a ground plane on both sides.
Through-hole parts with a ground pin will connect both planes.

Have a ground plane on both sides.
Through-hole parts with a ground pin will connect both planes.

That's my way of doing it as well, but using vias since I rarely use through hole parts. More complex 2 sided pcb's don't always allow for an unbroken plane.

Ok, originally I didn't move the ground plane to the other side because it wouldn't connect to ground on my top side, unless now as I understand, I add a via from the top to the bottom?

So I add a ground plane on bottom level...named it ground and hits the ratsnest button (had forgotten about that) and I got this:

Are the ground planes automatically connected somehow by EAGLE, or do I need to make a via for them to connect?

Also, how do I make my power traces and signal traces the right thickness all at once? Or do I have to select each trace one by one and change their thickness? I select a trace and right click and properties but I cant go past 0.254:

As for the mounting holes, here is the difference between the 3mm hole from the library vs a drawn circle. The issue with the drawn circle is that it only covers the top red layer for some reason and I cant seem to move it to the bottom blue layer:

How do you plan on programming this board?

I'm not an expert on this, but I thought you needed SCK, MOSI, MISO, RESET, Vcc, and GND. I'm not sure how well SCK is going to work with 5v on the pin via the resistor, and I thought a pullup on RESET was , while not mandatory, highly recommended. MOSI is also connected to a speaker.

Have you breadboarded the whole circuit and programmed it to ensure it will work? Hate to see you go through all this and order something that won't work as planned

If I'm wrong on this, someone PLEASE enlighten me.

Just name both planes GND, and parts with ground pins (the chip, speaker, conector) will connect both planes automatically. Putting a via in a not flood-filled area, and naming it GND, will fill the area.

You could still make the board 2/3 of it's size by..

lowering the speaker a bit
rotating R1 to a horizontal position and lower it towards C2
moving CN1 on the right hand side of the speaker
moving X1 next to CN1

The screw hole part should ofcourse (just) go inside the outline.

I did breadboard it and perfboard it, but I see your point, I never tried the programming of the tiny on those prototypes. I would program it by removing it and placing it on another breadboard I have.

Ok I see your point. I need to add the pullup resistor to the reset pin and what should I do, add a switch along that long diagonal from SCK to the Resistor?

Thx for the heads up!

You can add a switch or just a simple jumper that you can remove to program. On your board, you just need a set of header pins .1 apart.

As for the reset resistor, you might want a button on that. It's easy enough. Use a 10k resistor from +5v to the reset pin. The button then gets connected from the reset pin to gnd (or anywhere in between the pin and the resistor)

The gnd plane on the front and back may/may not be fully connected just from any through hole gnd pins. You have to verify this. It's an easy mistake to have a component grounded to the plane, then miss that the plane is broken (island). If needed, vias can be used to connect them.

Ok I added a jumper in the schematic. I wasn't sure which to add, so I added this one:

I had also added a via last night, but per Wawa's solution I removed it. I clicked ratsnest and it cleaned up the area it had cleared up around the via, cool!

As for the pull-up resistor and push button I added this to my schematic:

And what about the screw holes, which should I use?

Are you going to use the mounting holes? A .120in hole will allow a number 4 machine screw for mounting. I think 3mm is rather large for this project, but it's YOUR project.

I never found a library part for holes, so I always draw them by hand. The one you found looks good. I would use that.

Also, how do I make my power traces and signal traces the right thickness all at once? Or do I have to select each trace one by one and change their thickness? I select a trace and right click and properties but I cant go past 0.254:

1/4 inch traces are pretty damn wide. Wider than that, draw a polygon instead of a regular trace. I've used polygons for high-current traces where I need them to flow between the pins of other components.

To change all at once, define the net class for power traces. That's not very practical for this simple board. I have used that feature but it's not useful until your project gets really large.

The other way to make bulk changes is to use the Change tool, which looks like a wrench or spanner. You can pick a width and then just click on each trace you want to change.