17
\$\begingroup\$

Below is the schematic of the Pololu A4988 driver board:

Pololu A4988 driver carrier

There are three capacitors on the motor power input. I can understand why engineers decided to use separate 4.7 µF with larger size (1206, 0.1 µF are either 0805 or 0402): because physically small capacitors have lower ESR, and they effectively filter out higher frequencies (correct me if I'm wrong). But what is the reason to use two 0.1 µF capacitors in parallel? Can they be replaced by a single 0.22 µF in order to save PCB space and cost?

Image of the board; it can be clearly seen that all capacitors are ceramic:

Board assembly

\$\endgroup\$
3
  • 2
    \$\begingroup\$ Typically a BOM optimization. Is that C6 0.22 uF an electrolytic? Otherwise it’s a mystery. \$\endgroup\$
    – winny
    Commented Jan 3, 2020 at 10:27
  • 4
    \$\begingroup\$ @winny no, all capacitors are ceramic. I've added photo is the board \$\endgroup\$
    – Zhenek
    Commented Jan 3, 2020 at 10:41
  • \$\begingroup\$ tl;dr Because badly drawn schematic. They didn't follow our guidelines for drawing schematics. \$\endgroup\$
    – Nick Alexeev
    Commented Jan 5, 2020 at 2:04

2 Answers 2

Reset to default
35
\$\begingroup\$

C2 is used to decouple pin 28 and C3 is used to decouple pin 22 (or vice versa): -

enter image description here

See also the Allegro data sheet for the A4988 driver; it shows the capacitors as C7 and C9: -

enter image description here

\$\endgroup\$
11
  • 6
    \$\begingroup\$ Well, when I first looked, it was apparent to me that C2 and C3 are very likely to decouple pins 22 and 28. I guess experience of laying out PCBs for microcontrollers is an important thing and, on many circuits I’ve come across, all the “chip” decouplers have been drawn in a separate block so as not to clutter the more useful IO connectivity of the diagram @foreverska. \$\endgroup\$
    – Andy aka
    Commented Jan 3, 2020 at 18:53
  • 5
    \$\begingroup\$ @foreverska The OP's diagram is a schematic. It shows a logical layout of the circuit, not the physical layout. Since C1 C2 C3 and C6 are "obviously" power supply smoothing, they are drawn so they don't clutter up anything else. The drawing on the left of Fig 5 is the physical layout of a circuit board, and the circuit on the right is arranged to make it easy to compare with the board layout. Compare the way the outputs OUT1A, 1B, 2A, 2B are shown on the different layouts for example. The OP's diagram shows they all to the same connector. Fig 5 shows their physical position round the chip. \$\endgroup\$
    – alephzero
    Commented Jan 3, 2020 at 19:01
  • 2
    \$\begingroup\$ @foreverska It's fairly typical to have power supply decoupling capacitors grouped into one location in the schematics. The fact that they are grouped there indicates they are power supply decoupling caps. In large designs, it's possible to have an entire page of the schematics, or even more than one page, devoted entirely to power supply decoupling capacitors. While the schematics here could have a note indicating the purpose of these caps, personally, I found the fact that they are decoupling caps to be instantly recognizable from multiple indicators. \$\endgroup\$
    – Makyen
    Commented Jan 3, 2020 at 19:10
  • 3
    \$\begingroup\$ @alephzero: that kind of justification / explanation of different styles / priorities in drawing a schematic would make a good answer, or could be added to this answer. That's exactly the kind of well-known to people in the field thing that you don't get from just knowing physics and how to read a schematic, and that clears up the mystery of why you'd draw it that way. \$\endgroup\$
    – Peter Cordes
    Commented Jan 3, 2020 at 19:13
  • 1
    \$\begingroup\$ if the schematic would consistently show logical and none of physical layout, the the dookwise, uh, clockwise indicator label on the pot is certainly an exception to such rule. \$\endgroup\$
    – dlatikay
    Commented Jan 3, 2020 at 20:05
22
\$\begingroup\$

It is normal to use one de-coupling capacitor for each power pin.

Now you could place these capacitors all over the place in the schematic, but it is easier (and has become a sort of convention) to place them all together somewhere in a corner of the schematic where they do not interfere with the rest of the circuit.

Here is another example I have cut and pasted a bit:

Enter image description here

At the top you see three capacitors connected to 3V3 next to four capacitors connected to VDD_core.

Below that you see the CPU which has three 3V3 input pins (shown at the top), and I have pasted in the bottom of the chip where you find another four input pins which need to be connected to VDD_core.

Thus each power input pin as matched up with one decoupling capacitor.

In this case the CPU has an internal supply (a linear regulator) which provides the VDD_core power: the VDDOUT pin. Because it is an output of an LDO, it has a separate, bigger, 4.7 µF decoupling capacitor.

\$\endgroup\$
0

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service and acknowledge you have read our privacy policy.

Not the answer you're looking for? Browse other questions tagged or ask your own question.