Geting a female USB-A connecter to not hang off the board

Archive BatchPCB
1

On a small board that I’m designing (a USB iPhone charger) I have to put a USB-A female connector that hangs off the edge of the small board. The connector intentionally hangs off the board’s edge so I do not want to change the position but I want to keep the silkscreen/holes. The problem is that when I put this onto the board the way that I need it, the connector is counted in the size of the board, bringing the price of the board up $2.50. I would like to keep the price of the board down as much as possible. Is there a way that I can just take out the silkscreen that is sticking off the board?

Here is a picture:

http://img372.imageshack.us/img372/7199 … rorjk0.jpg

2

Modify the silkscreen for that component?

Leon

3

Jeremydeath:
USB-A female connector that hangs off the edge of the small board.

…

the connector is counted in the size of the board

…

Is there a way that I can just take out the silkscreen that is sticking off the board?

Looks like you're using EAGLE?

One solution is to create new outline packages

in the component editor, that only extend to the

PCB boundary. I had to do this with switches

and a digital encoder shaft for exactly the same

reasons as you.

If you’re unfamiliar with editing the component libraries

post you EAGLE files (*.sch and *.brd) for assistance.

BTW, you’re general PCB layout looks good but a

few of your traces seem too thin and too close to

other pads. Have you run ERC and DRC yet?

4

The routing is very untidy; boards look more professional if tracks are orthogonal or at 45 degrees, and non-circular pads shouldn’t have connections at an angle. Bigglez is right about the narrow tracks.

Leon

5

I agree with bigglez and leon, the traces are way too thin (i’d use 20 - 40 mils) and with a little rearranging

you could easily make it a single sided board… You didn’t say if were going to use Batch-PCB for this design

so going for single sided board may drop the price a bit.

(You could always switch to surface mount parts too… I rarely use the EAGLE autorouter but when i do, i

always use the ripup tool and relay the traces one by one… :roll: )

6

Ok thanks for all the help. I’ll try to fix some of the problems and to redo the silkscreen of the USB connector. I’ll post the picture when I’m done.

-Jeremy

Edit:

Here’s the finished picture:

http://img338.imageshack.us/img338/3491 … jpgkg4.jpg

I changed the traces to 32mils, routed the board by hand, only used orthogonal and 45 degree traces and ran SparkFun’s DRC. I rearranged all the components and was able to get the board down to 1.45 in. X 1 in. Does anyone have any more suggestions?

7

100X better! I will say that topside traces under a 7805 make me nervous, you’re depending on a very thin layer of solder mask to prevent a short. Looks like you can put those traces on the bottom with no difficulty.

8

Thanks for the tip. I didn’t really think about a short between the 7805 and the wires. Ill change them and the one under the USB to the bottom layer. Thanks for all the help. :smiley:

-Jeremy

9

The two blue tracks on the left look a bit untidy, with those kinks in them, and I’d chamfer the right angles. It does look a lot better, though.

Leon

10

Jeremydeath:
Does anyone have any more suggestions?

I haven't seen your schematic yet, but I'm

wondering why the LED has two ballast resistors

in series (R1, R2). You only need one, right?

11

Excellent, gazillion times better :smiley: . Take macegr and leon’s notes and your done…

(a little idea from me, if you confirm the tab of your regulator is at ground potential and moved the

output trace, you could create a ground pour which would delete the trace under the connector and

if you switched the connections to R2 then you might be able to put the blue traces on the same

layer as the others… Plus it would dissipate some of the heat :wink: )

After all that there is no need to do it, just an idea…

bigglez, the LED is powered from the output of the regulator, through R1 to ground.

And looks like R2 and R3, R4 and R5 make a couple of voltage dividers…

12

I cleaned up some of the traces and rounded one of the corners of the board. For the curious, here is the schematic.

http://img383.imageshack.us/img383/8044 … ticgg2.jpg

It regulates 9V+ to 5V and then splits it through a voltage divider into 2.1V and 2.9V into the D- and D+ pins of the USB. This is needed for the iPhone to accept it as a valid charger. Also there is a switch so that the battery isn’t constantly drained and a LED indicator. Every thing fits into a Altoids tin as a portable charger.

13

Jeremydeath:
It regulates 9V+ to 5V and then splits it through a voltage divider into 2.1V and 2.9V into the D- and D+ pins of the USB. This is needed for the iPhone to accept it as a valid charger.

Thanks! that explains the circuit well. The interesting

thing is you are missing the capacitors required by the

voltage regulator for stability.

See the [LM7805 datasheet and this thread ([Vreg discussion).](LCD Display w/ ATtiny2313 - SparkFun Electronics Forum)](http://www.national.com/ds.cgi/LM/LM7512C.pdf)

14

You might also want to add a couple of diodes in there.

A series diode on the 9V input just in case someone attaches the battery the wrong way around. If they did, hopefully it would only damage the regulator, but it’s possible it could damage the phone.

Also, another parallel diode across the regulator (cathode on input, anode on output). I’m not sure how the iPhone works with regards to charging, so this may not be needed, but the regulator will die pretty rapidly if the output voltage is ever higher than the input voltage, which could happen if the charger is attached to the phone without the battery present. This diode prevents that from happening.

15

Thanks for all of the ideas. I added the capacitors across ground and the input and output of the 7805. I looked up the spec for this part and the capacitor sizes indicated there were a lot smaller than the 10uF/100uF ones in the rule of thumb post (the ones on the spec were only 0.1uF and 0.33uF). I ended up going with the smaller ones because they fit on the board better. Also, I’ve pretty much run out of room on the board because I changed the switch type to something cheaper and that would handle the current draw better than the other one. Unfortunately, it’s almost twice as big so I don’t have enough room left for the diodes if I want to keep the board at $5 (< 2 sq. in.) with BatchPCB. It looks like the iPhone doesn’t try to draw power so I’m not too worried about leaving off the parallel diode across the regulator. Thanks for all the help and critiques. I’m pretty much finalized on the design. Hope this works.

-Jeremy

16

Jeremydeath:
I looked up the spec for this part and the capacitor sizes indicated there were a lot smaller than the 10uF/100uF ones in the rule of thumb post (the ones on the spec were only 0.1uF and 0.33uF). I ended up going with the smaller ones because they fit on the board better.

Correct. The datasheet shows the bare minimums.

Some vendors boast that no caps are required at

all with their versions of the regulator. Any capacitor

is better than done!

Is your 9V battery the [common type

found in smoke detectors and similar apps? I’m

wondering how many iPhone recharges you can

get out of one of those?

The iPhone (gen 1) has a [stock 1400mA-hr battery,

yet a 9V disposable battery is only 625mA-hr capacity.

Your circuit is not much better than 5/9 or 55%

efficient due to the linear regulator. Doesn’t look good…](iPhone Battery Replacement Kits & Services)](Electronic Components and Parts Search | DigiKey Electronics)

17

Trip down random energy calculation lane (warning, may contain errors):

625mAh * 9V = 20k joules

20k joules / 5V = 1100mAh

1100 * 0.5 = :frowning:

I think you could do better with two AAs, and a high efficiency boost converter to get 5V. Or 3 AAs.

18

bigglez:
Correct. The datasheet shows the bare minimums.

Some vendors boast that no caps are required at

all with their versions of the regulator. Any capacitor

is better than done!

I should have pointed out that the IC vendor is

striving for stability (no oscillation of the Vreg IC),

and only small caps are required for that task as

long as they are very close to the regulator pins.

The larger caps are to reduce the impedance of the

input and also the output for transient loads, which

would cause glitches on the power rails.

Modern electrolytic caps are superior to older

types, and can also contribute to HF (spikes and

pulses) that used to require parallel connection

of an electrolytic and small ceramic RF type.

19

I just uploaded a design of my own that has two RJ45 jacks that hang off one edge of the board. This board is the exact same size as another one of mine, they mate or stack on top of each other, and when the DRC bot ran it cut off the part of the connector that overhangs the board. The two sizes of the boards match exactly. I am using BatchPCB to make my boards.