sim900A based PCB project

[dizgah]

hi every body
im trying to make a pcb for sim900A gsm modem & stm32 mcu & some other parts.
i have some unsuccessfull experiences with that.i attached my new pcb project in altium designer 2015.
if any body can please check it and share with me his/her viewpoint.
best regards & thanks a lot.
pcb project:
https://www.dropbox.com/s/0emi4dc2iytrezt/PCB-PROJECT.zip?dl=0

 

[ArticCynda]

A few remarks:
- Why is the switcher (U2) using an adjustable inductor?
- Where is the feedback going? This needs to be as short as possible, so don't route the feedback to an external connector.
- You're missing a bead and a fuse on the USB power input
- A top level schematic is missing in your project
- The loading caps for the STM crystals are far too high, typically they should be between 15 pF and 27 pF
- Don't use a 2N3904 for on/off applications, instead use a 2N7002 N-MOSFET which is better suited and doesn't require so many resistors
- Decoupling caps for the STM should be 100 nF instead of 100 pF
- Consider using a resistor array instead of individual 1k resistors as pullup/pulldown on the JTAG connector
- The speaker lines should probably not be differential pairs

Good luck!

 

[dizgah]

dear ArticCynda
u2 is adjustable because sim900 supply with 3.8V & element p7 is a potentiometer for adjusting this parameter,it feedback output Voltage to the IC,(my pot's footprint is different form altium's one )
about your advise i will correct them soon & thank you a lot
this is project with pcb file , whats your recomms about that ?
best regards


- - - Updated - - -

uploaded in eda board.
excuse for rule violation

 

[FvM]

The STM32 power and ground wiring is horrifying.

This circuit part has to be rerouted, starting with all STM32 ground pins connected to a common ground pour and bypass capacitors next each power pin, directly connecting to the same ground pour

 

[dizgah]

your opinion about gnd pins is completely true, but about limitation of layers (my pcb has only 2 layer ) i cant design better one,
my emphasis is in sim900 part,because i have some unsuccessful Experiences with sim900A's pcb,none of my sim900 in last pcbs dos not work correctly & i want to be trustful of its correctly operate.
tnx any body

 

[ArticCynda]

I believe you're making this hard for yourself by using large through hole parts in combination with fine pitch surface mount parts like the STM32. Is there a particular reason why you're not opting for a standardized 0603 capacitor and resistor form factor? Since you have many identical values in your circuit, this would be much cheaper to manufacture and also make the board only a fifth of its current size or smaller (which again lowers the cost since you're paying for board surface).

I agree with FvM's remarks, you definitely need to redo the power routing of the 2 main ICs, it's unlikely it's going to work reliably without any decoupling at all.

 

[dizgah]

i am located in a small city & here finding SMD parts is more difficult than trough - holes.
i increase pad sizes because then i can remove parts after soldering & change them some times without damage to the routes.
routing without those vias in 2 layer is so difficults
awaiting for new observations
tnx

 

[FvM]

I believe you achieve better power and ground routiing on two layer PCB.

 

[ArticCynda]

i am located in a small city & here finding SMD parts is more difficult than trough - holes.

I'd recommend you to buy an SMD resistor and capacitor kit on AliExpress, for example this one: https://www.aliexpress.com/item/060...nents-Package-Samples-kit-free/811561691.html
It's easy for prototyping, you can make quite a few boards with them, and they can be refilled with standard 8 mm tapes. Choose a size (I'd recommend 0603 or 0805) and then stick with it, that makes the logistics of projects a lot easier.