Charger Layout!

Go To Last Post
15 posts / 0 new
Author
Message
#1
  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

Hi Everyone,

Please critique this PCB layout for me...this is a battery charger (LTC4060) and the output goes into a DC-DC converter (Max8815A). Please disregard the configuration of the power input, power output, and battery connection. All of these will change before I send this to AC. My concern is the power output IC is so small and I am worried about sinking the heat (to say nothing about whether or not I will be able to solder this baby. I think Maxims entire "Line Card" will fit in an empty cigarette box!) I have tried the "Carl" one side only method could not do it here. I have moved parts a zillion times trying to improve the layout. It should be noted that this board measures 1.125 x 2.25 inches!! The Max8815 is said to be capable of 5 volts at 1 amp!! I will only need about 300 ma!!

Thanks

John

Attachment(s): 

Just some guy

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

Some thoughts.

I would try and indicate polarity a little bit better on your diode footprint silkscreen.

You also look to have routed your ground quite far away from everything, this is going to increase loop area, you should probably at least consider filling the area in.

The ground routing strategy that you have used looks a little poorly thought out - surely your CT, Rp, C3 and C2 should ground more locally to their respective ICs then simply tap into that feed you have along the bottom of the pcb.

I really suggest you re-layout this design completely if you want to do it properly. Not settling on power connection points is also going to do you no favours as it will somewhat influence layout in the later stages.

You should look for some layout suggestions in the datasheets of the ICs you have selected and probably do some more reading on the fundamentals of DC:DC with respect to high current tracks and loop areas.

Best of luck.

oddbudman

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

Read >> this << document.

Most LT datasheets have example layouts and hints.

I would use the bottom of the PCB as one big heat sink and ground plane. With bit of effort you can keep all traces on the top layer. Don't forget to add proper heatsinking areas to the charger power transistor. Use lots of via's to carry away heat.

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

The board seems kinda.... empty?

Also, what kind of package does IC2 have? I don't think that it would be wise to put a big via under it if it has some kind of solderable bottom.

See: http://datasheets.maxim-ic.com/e... and http://www.linear.com/pc/downloa...

Under both ICs there are no holes.

There are pointy haired bald people.
Time flies when you have a bad prescaler selected.

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

But you need to solder that little pad on the bottom of the IC to a pad to carry away heat. If the board is not going to be oven soldered, there is no way you can get it soldered. A few via's will solve this problem. Been there, done that ;)

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

Thanks guys!! I will redo!!

David, I placed the holes under the IC's for access to soldering the ground planes on the bottom of the chip. I am still considering many options for "which" method I am going to use to solder these devices!!

I will re-post after my revision. This is the first time I have tried to use large copper areas - instead of - traces with FreePCB!!

John

Just some guy

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

Wow, JayJay...that is a great document!! Thanks so much!!
John

Just some guy

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

Here was my first attempt where I tried to lay as much copper as possible. Unfortunately the Gerber's kept adding thermal reliefs to the SMT pads even after I changed the setting so I abandoned this one!! Just thought I would share!!

John

PS: You will notice this version is called, "Please don't leave me!" That is what I saved it as after my latest "unstable" version of FreePCB caused me to execute a system restore to recover it!!! Oh Boy!!

Attachment(s): 

Just some guy

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

Considering the width of the other connections, shouldn't a very important connection (the one to L1) be just as wide?

There are pointy haired bald people.
Time flies when you have a bad prescaler selected.

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

Yes David, you are correct but, the struggle I am having is in keeping the trace width within the limits of 8 mils when the adjacent pins are so close!! The photo shows an actual size "top copper" gerber in an effort to show the microscopic chips I am using! Maxim has some really great stuff and their customer service is awesome but, all of their hardware is soooo puny!!!

This will definitely be a learning experience!!

Thanks for your input!! Is this second (actually first board) any better?? I could try to work out the thermal relief problem. With class every night this week I wont be able to work on a redo until the weekend!!

John

Attachment(s): 

Just some guy

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

You should keep the traces very wide, and then within, say, 10-25 mils, neck it down to 8 or 10 mil when you connect it to the little pin of the IC.

It looks like one side of the inductor connects to a corner pin of the IC, you can make this a big copper area, no need to have a small track. Heat is carried away from the chip via the pins, not the housing, especially the ground pin.

I usually route these circuits with copper areas, not traces. So you want as much copper as you can to act as a heatsink. The only problem with big copper areas is that soldering can be more difficult.

I prototyped with these little ICs on standard .1" through hole breadboard; some pins soldered to pads, other pins bent up with little wires soldered onto them.

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

1. Identify the tracks that will carry heavy current and selectively increase their width.

2. Identify the components that will dissipate heat and increase the amount of copper around those pins.

The transistor (I'm assuming that will be the biggest heat producer) could be turned around so the centre tab (collector/drain) can be more effectively heat-sinked.

Keep in mind that it is possible to use small value/ zero ohm resistors to jump the tracks and thus achieve single-sided nirvana.

If this is going into a case and you are allowed to have holes in it, think about air flow over the board. Convection cooling, based on the simple principle that hot air rises, is very effective and cheaply done.

If you think education is expensive, try ignorance.

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

Jay Jay's document is only viewable by 10 people:

Quote:

This file is neither allocated to a Premium Account, or a Collector's Account, and can therefore only be downloaded 10 times.

This limit is reached.

To download this file, the uploader either needs to transfer this file into his/her Collector's Account, or upload the file again. The file can later be moved to a Collector's Account. The uploader just needs to click the delete link of the file to get further information.

 

"We trained hard... but it seemed that every time we were beginning to form up into a team, we would be reorganized. I was to learn later in life that we tend to meet any new situation by reorganizing. And a wonderful method it can be of creating the illusion of progress while producing confusion, inefficiency and demoralization." Petronius Arbiter, approx. 2000 years ago.

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

Quote:
Keep in mind that it is possible to use small value/ zero ohm resistors to jump the tracks and thus achieve single-sided nirvana.

Forgot all about those!! Thanks!

Quote:

I prototyped with these little ICs on standard .1" through hole breadboard; some pins soldered to pads, other pins bent up with little wires soldered onto them.

Show off :lol: I will try!! I would like to try reflow on a hotplate...not sure I am up to the challenge!! Also, I feel that the 3 for 33 specials I get from AC never have enough solder in the SMT pads to reflow...is there a common amount that needs to be specified??

Thanks
John

Just some guy

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

My LT document reuploaded here. Should allow more then 10 downloads.