Continue to Site

Welcome to

Welcome to our site! is an international Electronics Discussion Forum focused on EDA software, circuits, schematics, books, theory, papers, asic, pld, 8051, DSP, Network, RF, Analog Design, PCB, Service Manuals... and a whole lot more! To participate you need to register. Registration is free. Click here to register now.

sim900A based PCB project

Not open for further replies.


Member level 5
Nov 8, 2009
Reaction score
Trophy points
Activity points
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:

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!

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


  • SIM900A
    1 MB · Views: 65
Last edited by a moderator:

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

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

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.
  • Like
Reactions: dizgah


    Points: 2
    Helpful Answer Positive Rating
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

I believe you achieve better power and ground routiing on two layer PCB.
  • Like
Reactions: dizgah


    Points: 2
    Helpful Answer Positive Rating
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:
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.
  • Like
Reactions: dizgah and FvM


    Points: 2
    Helpful Answer Positive Rating


    Points: 2
    Helpful Answer Positive Rating
Not open for further replies.

Part and Inventory Search

Welcome to