Is my LM2596 PCB design awful or not? +Questions about capacitors

[Tuppe]

Hello!
I'm currently designing my first PCB and I already went way out of my skill level with the low space. I'm using LM2596 switching regulator circuit, with full circuit listed in my IC datasheet. It powers SIM908, which is using mostly 5mA current and peaks to max 2A.
Input is 12V-15V from car battery.

So here it is(apologies of my poor paint skills, my cropping efforts to make it simpler might've made it more convoluted):

Schematics should be correct(SIMCOM datasheet refrence in black & white), but how awful is the design? Should I scrap the whole thing, or does this have a change to actually work? I've really struggled to get it fit with my previous design.

PCB design questions:
1. There's no GND path across the blue line to white area, so is the GND path insufficent? Does the GND connect through the LM2596(marked to image)? I have GND bottom layer, in which I plan to take few GND vias.
2. Is placement of the components good enough? I tried to stick to instructions keeping filter and adj. caps close to the LM2596.
3. Is trace width/layout sufficent?
4. Is overall design sane at all?

LM2596 Capacitor question, I've read numerous articles about filter capacitors, but every source seems to tell differently. Those components in the Eagle board are based on Ebay LM2596 design.
1. Tantalum, electrolytic or ceramic? Some say tantalums can't handle the voltage spikes, and some say they last longer. I want it to be as reliable as possible. I'm not into saving few cents. Nippon or Nichicon all the way. Some sources state that ceramic are only ones with low ESR(obviously I can go ceramic on the 330uF, but the other ones). Some seem to go with aluminium.

For inductor, I've chosen typical 100uH SMD 3A closed core inductor. I think that should be fine.

Thank you very much for reading!

EDIT: Oops, ignore the below attachement, I enhanced the image a bit and I can't remove this old one.

 

[FvM]

MBR0520 is a 0.5 A diode, it may be used, if the average output current is clearly below 0.5 A and rms not much above 0.5 A. Also trace widths won't be good for more than 1 A rms. A GSM module might slightly exceed the diode rating in high speed GPRS operation.

I won't thermally isolate the LM2596 ground tab, rather provide additional thermal vias to use top and bottom copper as heatsink.

 

[Tuppe]

I definitely need to swap it to 1N5822 and thermally connect the ground tab. As you said about the thermal vias, I only now realized, that all those perforated tabs were for thermal connection. I definitely use that method, although it's sleeping so much of the time, that I wouldn't think it would heat up at all, because neither does linear regulator.

I calculated that with 1oz/ft² copper, I can use 30mil traces where the max trace length is 10mm: https://www.desmith.net/NMdS/Electronics/TraceWidth.html
I used mostly 32, but under the LM2596 I used 24. I guess I can widen the trace below the module ground tab.
I can use wider in the most areas, so I will definitely go as wide as the pads allow. I'm not sure did I mess up with the mm/mil units somewhere though.

I was more conserned with the trace meeting LM2596 operation specification. Datasheets seem to state merely guidelines rather than strict limits.

Thanks for the input. I guess there isn't anything horribly wrong with the overall layout? I was thinking I could spin that INPUT CAP around, to minimize the trace length to LM2596.
Any ideas for the capacitor types? Are those aluminum ones the way to go?

 

[FvM]

Particularly the input capacitor must be a low ESR type, because the input current of a buck converter is discontinous. If you have difficulties to find a suitable low ESR capcitor, you can also use larger ceramic capcitors in parallel, e.g. 10 µF.

Output capacitor ESR affects the ripple voltage and might be critical too, depending on the GSM module specification.

 

[Tuppe]

I don't think I have the space to fit multiple capacitors in the board.

Problem with the "low ESR" specification is that I don't know where is the actual limit. Datasheet lists Nichicon PL, but I can't find 100uF and 330uF from Ebay(free shipping is a must).
Many seem to use tantalums with same module, but if there's any change they can blow up, I won't risk it and I don't see anybody would use them. Especially with car circuit, where very high voltage spikes may occur.

I can find lots of these "motherboard capacitors", are these any good? I've no idea what RMS ripple range should I aim for.
**broken link removed**

All the LM2596 boards seem to use SMD capacitors, but if they work the same, I can go with either. I can't really find branded +25V SMD caps for the exact 100uF and 330uF values.

 

[FvM]

I don't think I have the space to fit multiple capacitors in the board.

I would normaly agree that this may be a reason, but your layout has pretty much of free space.

Unless you are making a production design dedicated for automatic assembly, I won't use SMD electrolytic capacitors. There's a reason why PCB motherboards are still using regular radial capacitors, at least the price.

I won't use tantalum caps, except for polymer tantalum on the low voltage size, if you are going for utimate low size.

 

[Tuppe]

I would normaly agree that this may be a reason, but your layout has pretty much of free space.

The image is actually cropped to simplify the area in guestion. There's all around components immitiately to the left.

Unless you are making a production design dedicated for automatic assembly, I won't use SMD electrolytic capacitors. There's a reason why PCB motherboards are still using regular radial capacitors, at least the price.
I won't use tantalum caps, except for polymer tantalum on the low voltage size, if you are going for utimate low size.

I assemble this by hand, 5-10 units at most, so the choice really comes down only in experience of component selection. I've yet nearly none of that experience.

Thanks for the tips, I will definitely switch my design to ordinary radial capacitors. I'm a bit surprised there was apparently so little wrong with the design.
I hope those Ebay ones aren't fake Nichicon.

 

[Mattylad]

Consider your GND return path and improve that GND return a lot.

Also ISTR that there are high switching currents in the diode, so rotate it and put it directly across the IC pins with the inductor in front of the IC and do not use the longer track from the diode to it.
Move the cap to the right to help achieve this.

The output should come from the cap+ not the inductor.

 

[FvM]

Also ISTR that there are high switching currents in the diode, so rotate it and put it directly across the IC pins with the inductor in front of the IC and do not use the longer track from the diode to it.

The input current is commutated between Vin respectively input capacitors and the diode, not the switch IC ground. In so far the return path isn't that bad.

 

[Tuppe]

Consider your GND return path and improve that GND return a lot.

Also ISTR that there are high switching currents in the diode, so rotate it and put it directly across the IC pins with the inductor in front of the IC and do not use the longer track from the diode to it.
Move the cap to the right to help achieve this.

The output should come from the cap+ not the inductor.

Thanks for the feedback!
Because I need to keep the inductor as far as SIM908 as possible, I decided to flip the whole power supply to improve on the details you mentioned.
With through-hole capacitors I was able to use space way more efficiently. With that I also chose to use through-hole LM2596 instead of SMD. I have plenty of room above the board. I'm really happy with that decision, that gives more room for the SMPS layout and way better GND path. I think it's way better now, but there still might be some new goofs.

high switching currents in the diode, so rotate it and put it directly across the IC pins with the inductor in front of the IC and do not use the longer track from the diode to it.

I'm not sure did I understand thins sentence correctly, but you can see the resoult in the attached image.
I though that it was only a flyback diode for inductor surges when switching ON and OFF. But I'm not so familiar with SMPS circuits.

You can ignore the traces in the rest of the circuit, it's just autorouted.