EAGLE dimensions/drill issue

I have this design:

which shows 2 types of error; Dimension for the power connector at the bottom and Drill Size for the 4 corner holes of the board Im designing.

How do I solve the drill size issue where I can see these options. Iow, how do I know what drill size to match it to?:

Change the design rules to allow smaller drills. The default via settings in Eagle use a smaller drill
diameter than the default design rules, but the design rule defaults are ultra-cautious, just change 24mil
to 20mil for the min drill size. You can change the dimension clearance down from 40mil too, I do.

BTW You have no ground-plane, your supply traces are too narrow, I see no decoupling cap(s) for the chip.

I must say those mounting holes are rather small. Smaller than any other hole on the board. Also, the ground trace on the battery terminal is rather odd, and that decoupling capacitor isn't close enough to perform it's function. It needs to be right by the power on the ic, not the isp header. You have run traces (too small) unnecessarily close to other pins, and as pointed out, you have no ground plane, which would solve some of the issues in itself.

If you have this board made, you are more than likely to end in failure, which isn't always a bad thing. It can help to teach, but having the failure caused by simple things can just be disappointing.

Thanks Mark & tinman,

  1. How do I change the min drill size from 24 to 20?

  2. How do I move the capacitor closer to the power input? I tried with the move tool but it leaves the trace bendpoints in place where they were originally.

  3. Where would be the best place to add the ground place, on the top, bottom or left/right?

I don't use Eagle, so I cannot tell you how to change the min drill size, but I would say to make those mount holes a whole lot bigger. Right now, they are pinholes.

As far as the capacitor, unroute the traces, move the capacitor, and place new traces in. I would get those traces a big bigger, and get them away from other pins. The traces at pin 3 and 5 have no reason to be that close to the pins. Just a little stray solder will short them, and I'm not sure the soldermask will adequately protect them.

The ground PLANE can be on both sides of the board, and will actually replace all the ground traces. The whole surface will be covered, except for the existing traces and a small area around them, which you can set. ^The ground plane will connect with the negative terminal of the battery, the ground pin of the ISP, the IC, the piezo, and anywhere else you have a ground connection.


  1. How do I change the min drill size from 24 to 20?

  2. How do I move the capacitor closer to the power input? I tried with the move tool but it leaves the trace bendpoints in place where they were originally.

  3. Where would be the best place to add the ground place, on the top, bottom or left/right?

There is an icon on the left side, down, called DRC. There you can change the design rules.
One of the tabs is Size/Minimum Drill.

Select what you want to do by right-clicking the mouse.
Move, or rip-up the track if you don't like it. Then re-route it.
On the top bar you can change layer, track width, etc.
Right-clicking while you draw the track changes track behaviour.

There is a "holes" group in the parts library.
You can use that to make mounting holes.

Draw two polygons on the board outline.
One on the top layer and one on the bottom layer.
Then name them GND.
That will flood-fill top and bottom (after clicking the ratsnest icon).

Post the eagle files (.brd .sch .pro) in a .zip file.

  1. By this stage you should have a good idea where you're going to get this manufactured. Download their design rules file and load that when you do the design rule check. (You only load it once, then it remembers all the rules which apply to this board.)

If they don't provide a downloadable Eagle rules file then you must enter all of their limits like minimum trace width and minimum hole size manually. Then save this as a file so you can use it again in other designs.

  1. Those holes are so small you can't get a wire through them, let alone a mounting screw. Look how tiny they are compared to the component legs.

  2. The "dimension" warning says that part of your component footprint (specifically the pads you solder it to) are too close to the edge or - in this case - overhanging the edge. Sometimes that's not a bad thing when you want copper all the way to the edge. In this case, it looks like you've chosen a surface-mount plug and you've mounted it with the opening of the plug facing into the board, not out.

Ok I unrouted and moved the cap closer. I have 2 questions:

  1. Is this close enough?

  1. Is this how I should change the drill size?

Screen Shot 2017-08-29 at 5.18.05 PM.png

  1. Third question...is that power connector placed correctly? I actually think I have it wrong. It looks like the copper connections are actually the dark red small rectangles whereas the knotch sticking out is where the cable connector will clip onto?

Screen Shot 2017-08-29 at 5.18.05 PM.png

  1. Is this close enough?

Not really. All you did was rotate it. The decoupling capacitor needs to be as close to the ic Vcc pin as feasible. In your instance, move your resistor down in line with the reset pin and place the capacitor where the resistor was.

Speaking of the resistor, I had just assumed it was a pullup for RESET, but a quick look at the ATtiny85 pinout says you have it hooked to SCK. That isn't right . Re-recheck your circuits.

As for the drill-size, Yep, that looks like where you would change the physical size.

As for question 3, I would guess you DO have it backwards. Do a 180 on it, and bring the positive trace similar to what you have. The neg lead will be attached to the ground plane you have to figure out yet. Same goes for ALL the negative/gnd traces. There won't be any.

Ok I changed the pins to 0.039. What are the units on that btw?

As for the cap, ok I thought you meant put the cap close to the battery in, thats why I moved it a tiny bit closer to the power connector. It makes sense that it be closer to the actual IC pin since that is who it would need to feed power to. So I moved it closer to the IC's Vcc and GND pins:

Screen Shot 2017-08-30 at 5.10.19 PM.png

Ok but that resistor is something Im using for the flex sensor, its required by the flex sensor.

I also figured out why sometimes I cant move components. Apparently some components are "off-center" from their cross-hairs. So when Im tapping over the component, my pointer is actually far from the crosshair, so its as if Im not selecting anything really. I need to move my pointer off to the side about a centimeter and the pointer will actually select the component. Weird!

Screen Shot 2017-08-30 at 5.10.19 PM.png

The units currently in use are defined on the "grid" settings. You can select mm, mils (thousandths of an inch) and maybe other options. It's an odd way to do it but that is how Eagle does it.

Parts are selected by clicking their "origin" which is the little "+" near the middle of each part. It doesn't have to be the middle. Sometimes a library part will have the origin on pin 1 or anywhere. Text on the PCB or schematic also has an origin - usually bottom-left but it's selectable in the text properties.

Origins are actually on a layer of their own. If you turn off that layer (so you can print the schematic or PCB without the "+" everywhere) then you can't select any components because the origins are invisible.

Another useful tip: Make sure the name of the project and a date are printed on the sikscreen on the PCB. I also add a version number and my own name. It helps keep track of multiple versions of PCBs.

You still are not following what the capacitor does or where it should be physically located. You moved it up, but it's on the wrong side of the ic, and instead of being routed to the Vcc pin of the At85, it is routed to the ISP header first, then to the Vcc pin. That's a long way to be very effective. The capacitor needs to be where the resistor is. Move your resistor down. Are you sure your capacitor has .1" leads? Just picking something to put in there out of the list with no real idea of what it is leads to problems.

As for the SCK/ADC1 pin, you have ADC2 and ADC3 unused on the other side of the ic.

Changing the mounting holes to .039 still isn't helpful. They are still very, very small. So small, you won't find a screw to fit it at any store around you. Perhaps something in the .130, which would be similar in size to the mounting holes on the Uno.

Ok I could only find as high as 0.12598 but I figure thats close enought to 0.13?

As for the cap...well Im not sure why it got ratnested that way. This is my schematic:

I meant to moung the cap near the IC, but that doesnt translate to the board and I guess it kinda makes sense because the schematic IC doesnt really have the Vcc and GND pins on the real sides, it actually has them both on the same side, which just isnt true. But ok, so how should I make the IC's Vcc wire connect directly to the cap first and then to the ISP header?

You can just type in a value for a hole size. You don’t have to pick one from the list. For large-scale manufacturing, it may make sense to restrict hole sizes to a limited number of drill bits, but prototype manufacturing uses routing to cut out larger holes with a small tool.

The ratsnest is irrelevant. What matters is the tracks you (or the auto router) draw.

Well I have moved the cap up next to Vcc pin, having moved the R up higher on the board. But auto-route moves the cap back down next to the power plug and isp header:

Don’t want to discourage you, but I think it looks terrible.
Parts need to be moved and rotated, so you have the least amount of crossing traces.

Example: rotate the speaker 180 degrees, so the blue trace can go left of the MCU.
Rotate C2 90 degrees anti-clockwise, so the blue line can go outside the ISP connector.
Or put C2 above the connector. etc. etc.

I never got a good result from the auto-router, so always do it manually.
Rip and re-route each trace.
Make them twice as wide.

Post the eagle files (already said that several posts ago).

I didn't know that the auto router could move parts. I must have that option turned off on mine.

It's turned the connector around again. I would not trust it any more. (Or you posted an old screenshot.)

You’ve aborted and reverted the autoroute I think. You have to End Job, otherwise the changes are reverted
since the start of autorouting.

Don’t use the autorouter, hand route, you know which signals are supply and need to be thicker, your brain
is much better at routing than the Eagle autorouter!

Here is the compressed folder attached below.

I have ripped up all traces with the ripup tool. I forgot how I did it but I think last time I figured out a way to rip up everything at once instead of clicking on each trace. After ripping up everything, I moved the resistor and cap into position but I think the ratnest lines would still be the path of choice that auto-router will follow. But ok, you say I should route the traces manually. Its kinda confusing with all those ratnest lines in there. Also how do I know which is +/- on a component:

So I came up with this so far. The Vcc doesnt look like it touches the pad on the power connector:

Flexie.zip (212 KB)