Tom,
I can't see any obvious reason for this not to work and, like AcHmed99, I wonder if you got a genuine part. If you can get TI to ship you samples or buy some from a distributor such as Farnell that might be better.
It's also worth testing it with a load of a 100mA just to establish that it is not a question of minimum load (though, as AcHmed99 says, the hysteritic control should be fine at low loads).
After being exposed to +15V (or worse), the output 10V capacitor is suspect [1]. This is not the root cause but it may be a secondary problem.
Conduct the remaining tests with at least a small load on the output (say 1kOhm, this will only draw a few mA).
Try the following observations with a x10 oscilloscope probe and a short ground lead to one of the output ground pins. Make a DC coupled observation and then an AC coupled observation with a higher sensitivity if nothing shows up on the DC observation:
The ground plane around pin 5 (SGND). This will give you an idea of how much things (including your observations) are bouncing around with switching noise.
Output voltage (you will see something on the AC coupled reading).
Input voltage, should be steady with a bit of ripple but check anyway.
Pin 7, BOOT. Ditto.
Pin 6, VDD. Ditto. Record the DC voltage.
Pin 8, the switching node. This should switch between ground and Vi+Vout (I think). Record max, min and frequency; get a screenshot if possible.
The anode of D1. Min, max, screenshot.
Pin 1, PGND. Compare this with pin 5. My guess is that this will look horrible (more on that below). Min, max, screenshot.
Pin 4, FB. Sticking a probe onto the feedback node of a working converter would be liable to screw the operation up, in this case that's less of a worry. This should be about a third of the output voltage.
If you see something funny, record the amount of funny [2].
Two things stand out in the layout. The first is the connection of pin 1 to ground. Pin 1 is the power ground that (according to the block diagram data sheet) handles the switching current. This should get a thick short trace to the ground plane/ bypass capacitors and be kept away from the feedback network. The example layout in the datasheet (figure 19) also shows a long thin trace that is shared with Rf2 of the feedback network! This is madness!
There is a picture of the boost circuit evaluation board -
http://www.ti.com/tool/lm2621eval - this is the board that TI actually built. It clearly shows pin 1 getting a short fat connection to the input and output capacitors. The feedback network is grounded at pin 5, signal ground.
I suggest moving R-f2. I think the easiest place for it is to bridge it between C1 and the adjacent ground strip.
Give pin 1 a connection directly to the adjacent ground via.
The second is that the output capacitor C3's ground current goes directly into the signal ground, pin 5. I suggest removing it and fitting a new capacitor between the output and the ground connection for L2; i.e. place it physically alongside D1 and make connections with copper foil, braid or wire to 3V3 and to the ground via for L2.
The aim is to connect things to PGND and SGND as appropriate and to reduce the area of the switching current loop.
However, this doesn't explain the behaviour described so I would start with a known good IC. Good luck and let us know how you get on.
[1] Tantalum capacitors are suspect when sitting brand new in their packaging, in my jaundiced opinion, but they're particularly suspect when they've been over-volted or reverse biased.
[2] I think this comes from Bob Pease?
Home
Help
Search
Login
Register
