Some help/advice for a board being built

I’m still new at making boards, and using Eagle in general. That being said, this circuit is intended to be a combination Lipo Charger and USB Charger rated at a maximum of 1A output. I’ll post the working schematic as well as a screen shot of my layout, just to get a feel for the circuit.

I’ve been using Sparkfun’s DRC file, and have gotten everything more or less sorted out.

Issues:

  • One of the chips that I’m using (MCP73833 for LiPo Charging) is of the form factor MSOP. Unfortunately, the Sparkfun design rules don’t allow spacings this small. I was wondering what DRC settings I should change to allow a chip of this size, and what complications this might cause

  • The board is small. This was on purpose. If you look at the picture, you’ll notice that it’s width is the same as the 2Ah Lipo Battery on Sparkfun. This is no coincidence. I’d like to put this in a box or some sort of container for travel and such.

  • I have not done any screening on this, as things still might change. General screening advice would be welcomed.

  • Since I’m still new at this, there are probably some things that I’ve overlooked. Any improvements and suggestions are completely welcomed!

A few things come to mind:

  • You should try to use as much of the bottom layer as a groundplane as possible, particularly under the switchmode circuit. You may have to add a few more vias to move tracks from the bottom to top layers.

  • Why no component identifiers on the silkscreen?

  • I always like to see protection against overvoltage / short circuit on pins that are accessible to the “outside world” (eg polyfuses & TVS). If you aren’t using “protected” lithium cells you’ll also need to think about protecting them against over-discharge. It’s normally better just to get protected cells.

The board has been updated. Consequentially, using the GND plane made routing a lot easier.

The symbol names were simply disabled.

Any ideas as to how I could alter the DRC rules to allow for the MSOP package? (Using Sparkfun’s file at the moment)

It’s much better now that you have a groundplane, but there are still a few important things to look at:

  • That inductor looks way too small. According to the LT1308 datasheet, the inductor needs to be able to handle at least 2A steady-state (see page 13).

EDIT: Actually, the inductor looks OK (I was looking at the wrong part!). However, you still need to follow the next point)

  • You really need to read and follow the layout guidance on Page 9 of the datasheet as closely as possible. Switchmode circuits can be quite important in this regard.

  • The component labels for most of the parts are way too small to be printed on the PCB

As for your question about the MSOP package, it has 0.5mm pitch leads, so I’m not sure why you can’t meet the 0.008" track / spacing requirement of BatchPCB. Why not make the pads 0.25mm wide, which would give a spacing of 0.25mm (ie, 0.0098")?

I didn’t give it a very thorough look - but what is going on with R4 being beneath D1?

[Board & Schematic Updated]

So it turns out that I was using Eagles default rules for the DRC. Switched to Sparkfun’s, and all was ok.

The inductor has changed accordingly. And to my surprise, the part that I was using was a tad to big. [This is the inductor that will be replacing the one I had on there previously (new dimensions are in the datasheet). It seems like it would do the job just fine, despite being small.

The board was redone with the new recommendations in mind, as well as some parts updated as well. I didn’t know that datasheets had this kind of useful information.

I know the text is still small. I’m still working on adding the silkscreen.](TSL0808RA-4R7M3R5-PF TDK | Mouser)

That inductor would do the job, but I normally prefer to use shielded type inductors, such as the following, since they reduce the radiated noise that such a circuit generates (I also like SMD inductors, but this is more a personal preference):

http://www.mouser.com/ProductDetail/Bus … QXpg%3d%3d

As for the layout of the switchmode circuit, I think you need to check the datasheet recommendations again. They show a continuous, unbroken groundplane under the entire circuit, which you do not have. This is important. On the top layer, instead of using tracks to connect the various components, they have used small filled areas (planes) to reduce the inductance / resistance and “loop area” for the high current paths.

If you’re planning to solder this board by hand, you may want to use “thermal reliefs”, but if you’re using a skillet / oven to solder, then do what they show, ie, solder directly to the planes.

[Board Updated]

I’m not sure if I understood correctly, but since the layout on the datasheet had a ground plane instead of routes, I went ahead and added a ground plane to the top layer of the board as well.

I’ve done most of the silk-screening for the components, using Sparkfun’s Eagle board as a guide.

I think I’ll stay with the inductor that I have, just because the SMD alternatives look a bit too daunting to solder for the time being. Perhaps after I see how well this inductor works, and have more experience soldering SMD parts.

zerotruths:
I’m not sure if I understood correctly, but since the layout on the datasheet had a ground plane instead of routes, I went ahead and added a ground plane to the top layer of the board as well.

In the reference design in the datasheet, there is a continuous, unbroken groundplane on the BOTTOM layer. The top layer is broken into small planes for the high-current areas, as discussed. In that design, there is only a small section of groundplane on the top layer, and this is tied to the bottom groundplane using a bunch of vias.

I highly recommend that you follow the reference design as closely as possible.

[Board updated]

Ok. So the board has been updated yet again. I changed the tracks to planes as much as possible on both ICs. I’ve also added plenty of vias to both IC’s ground planes. On the DC/DC converter, the vias minimize switching currents, and on the LiPo Charger they’re meant to better distribute heat to the back of the board, both of which were suggestions in the datasheets.

Some parts were moved around of course, and their silkscreens accordingly.

I have a feeling that this board is close to being completed for now, so I’d like to thank you for all of the help and advice that you’ve been giving me. I don’t even want to think how long it would have taken me to realize all of this information on my own.

zerotruths:
I have a feeling that this board is close to being completed for now, so I’d like to thank you for all of the help and advice that you’ve been giving me. I don’t even want to think how long it would have taken me to realize all of this information on my own.

No problem - happy to have helped. Looks good to me now.
  • Check your DC input jack; some of them have a ridge that has to sit at the board’s edge. Even if not, the face of the jack looks like it is recessed quite far from the board edge.

  • Label JP2 and JP3 with polarity

  • Label all connectors (other than USB) and LEDs with their function

  • Some refdes will be hidden by the components when they are loaded.

/mike

Thank you for the reminders. The outline for the jack assumes that the part is going to be placed slightly hanging on the edge of the board. I looked at this from the getgo and found that the jack that Sparkfun sells would indeed work. I’ve marked the polarities as well (something I meant to do, but almost forgot about). Cleaned up some of the text, and changed some names.