drawing schematic advice

Discussion in 'The Projects Forum' started by fran1942, Sep 6, 2011.

  1. fran1942

    Thread Starter Member

    Jul 26, 2010
    Hello, I am new to electronics and have tried to put together a schematic for a design I am working on.
    As this is my first attempt at a schematic can anyone please give any advice on whether this looks OK. I dont mean component values etc. I just mean the overall aesthetics and structural layup. Is there anything obvious I have done wrong or improvements I could make ?

    Thanks kindly for any help.
  2. mbxs3

    Senior Member

    Oct 14, 2009
    I would say that it is pretty good. I have no real experience with developing schematics but I use them all the time for my job and I would say that your schematic is on par with what the engineers are providing.
    fran1942 likes this.
  3. steveb

    Senior Member

    Jul 3, 2008
    Yeah, not too bad at all.

    You could neaten it up a little by using the ground symbol more often. For example, U1 pin 2 can have a ground symbol right there and then you don't need to drag the ground line around the whole schematic. Same thing with the speaker and other similar spots. Also, I see a couple of node dots missing, which appears just to be a typo. Also, some node dots are in weird spots, again a kind of typo, perhaps introduced by the software.

    Some personal preference things. I like to see Vcc pointing up when possible and the mic input on the left side of the schematic. Also, I don't like base connections that cut across the transistor symbol from the collector/emitter side. But, that isn't an issue of being wrong, it's just my preference. I've seen others do similar things before. Also, I've seen others use ground symbols pointing up or sideways which I discourage because it looks like an antenna to me. So, there are plenty of personal preferences out there, and don't let me rain on your preferences if you feel strongly about them. The greats in all fields have a tendency to break conventions when it suits them. :p
    fran1942 likes this.
  4. MrChips


    Oct 2, 2009
    As the previous two posts, not bad for a first attempt. As steveb says, we're not going to rain on your parade and beat you up too badly. There are some pointers to set you straight. It's getting late now so I will leave it for another time and I will get back to you with my tips.
    fran1942 likes this.
  5. tracecom

    AAC Fanatic!

    Apr 16, 2010
    As previously posted, there are several items that are a matter of personal preference that could approve the appearance of the board. The inconsistency with the use of node dots seems to be the main issue with regard to accuracy. An example is in the upper left hand area of the drawing where the two caps on the input and the output of the regulator are not technically tied to ground because the node dot is missing at the the junction of the two caps and pin 2 of the regulator. There are also some places where node dots are shown but not needed. Normally node dots are not needed unless there could be a question as to whether two or more wires are connected, and the node dots are used to indicate an electrical connection.

    And although you didn't ask, I do have some observations about your circuit.
    1. The two caps on the regulator are not what National Semiconductor recommends. NS recommends a .33 μF on the input and a .01 μF on the output.
    2. The serial download pin on the PICAXE chips must never be left floating. This will give unreliable operation. Always use the 10k/22k resistors as shown in the manual, even if the chip was programmed on a different board.
    3. There should be a .1 μF cap from power to ground on both PICAXE chips, located as close to the chips as possible.
    fran1942 likes this.
  6. DickCappels


    Aug 21, 2008
    In general, inputs on the left, outputs on the right, down to subcircuit level. Highest voltages toward the top of the page, the lower the voltage, the lower on the page, negative voltages treated similar to positive voltages, but mirrored about ground.

    Use ground symbols extensively, drawing in ground connections only when doing so clarify.
  7. Hi-Z

    Active Member

    Jul 31, 2011
    Yes, well done for a decent first attempt!

    A lot of good points have already been made, but I would say that I don't like the orientation of the Q1, Q2 circuitry. Ideally, this would have preceded the rest of the circuitry and been located on the left hand side, and would have had the (npn) transistors with emitters downwards. However, I realise this would have made the diagram too wide - but my preference for transistor orientation stands.

    Also, I know the point about missing "dots" has been made, but the situation of the two C1's either side of the voltage regulator demonstrates a pet hate of mine: the 4-way junction. Even with a dot, I think this is ugly and potentially ambiguous (as in "is there meant to be a connection there or is it just bridging?"). In general, I would avoid 4-way junctions - here I would avoid the problem either by connecting each capacitor down to the horizontal ground line or by using ground symbols.

    (By the way, C2 appears to be shorted out!)
  8. SgtWookie


    Jul 17, 2007
    You are missing current limiting resistors for LEDs D3 through D5.

    I don't know what you are using for Vcc, but there is only R5 between it, and pin 3 of the left PICaxe. You normally want to avoid situations where voltages on the I/O pins could exceed Vcc/Vdd or go below ground, as that could result in the uC being damaged.

    Meanwhile, you're using the Vcc label for the voltage coming in to the circuit from the left, but the Vcc required for the PICaxes is a regulated 5v that really should be called Vcc. I suggest that you re-name your input voltage from Vcc to something like V+ or Vin, and then label the output of the voltage regulator as Vcc. Otherwise, if you attempt to make a PCB from the schematic, the PCB software might try to connect your raw unregulated input voltage to the Vcc pins of the uC's - not a good situation.

    You seem to have D1 there for reverse polarity protection; but you're using power from before that diode to the mic amp circuit. If reverse polarity is applied to the circuit, the uC's might be OK, but Q1/Q2 might be damaged.

    I don't see any caps across your uC's Vcc and GND pins. While you don't necessarily have to show them on a schematic, you should make a note that all IC's have 0.1uF caps across their supply pins. These are required; if you omit them you will have problems.
  9. monster_catfish

    Active Member

    Mar 17, 2011
    Is this an iron-clad rule for all linear and logic IC chips, SgtWookie ? Also am I right in understanding that the caps are to be connected between Vcc and ground in all instances where IC chips of any description are used ?
  10. kubeek


    Sep 20, 2005
    Generally, all ICs should have them, but they are most important for digital and high bandwidth analog circuits. They will save you a lot of troubleshooting.
  11. SgtWookie


    Jul 17, 2007
    Yes, the 100nF/0.1uF caps across IC power pins are generally considered a minimum requirement. There should also be more of these bypass capacitors across the power rails sprinkled around the board. You should also have a larger electrolytic cap where the power enters the board. Many ICs require more than just a single 0.1uF/100nF cap. See the datasheets for recommendations.
  12. t06afre

    AAC Fanatic!

    May 11, 2009
    Not bad for a beginner I would say. As others have said. No need to skimp on the use of the power symbols like GND,V+,VCC and so on. I also noticed you have put the speaker directly to the output of the PICAXE chip. I do not know how wise this is. The PICAXE is just PIC microcontroller. And it have limited drive capabilities.
    You also have several capacitors named C1. And other are just labeled U?. You should annotate your schematic again. The capacitors connected to the 7805 IC. Is only connected together and not to GND. As you see it is no dot in the junction. It would also be better if you could use pdf files instead of a bitmap format. If you use newer versions of Altium Designer. You can print PDF directly from the GUI. If you use Protel 99 SE. Download a free PDF printer driver.
  13. ErnieM

    AAC Fanatic!

    Apr 24, 2011
    I've actually done just that, except I put a large (10uF? 100uF?) cap in series with the speaker to keep AC out of it. When driven with a PWM signal derived from a .wav file an intelligible sound was produced. Not high quality nor very loud but it was there. Should be fine for a beep or such. Add an amp if not loud enough.

    I don't see Q1 doing much since as drawn the base is connected thru C2 to the next stage. the gain there comes from the collector.

    Previous points about drawing Q1,Q2, and the LED sections well taken. I am having trouble "seeing" how these LEDs are controlled. A great schematic has a flow that can be followed in an intuitive sense, which of course cannot be taught, must be grown in your brain from experience.

    I've seen far worse from "professional" draftsmen, this is a very good start.
    fran1942 likes this.
  14. SgtWookie


    Jul 17, 2007
    If you are planning on using an electret mic, you will get rather poor results from your transistorized circuit.

    Consider using something like this instead:


    But if you're planning on operating on low voltage, you'll need a more modern opamp than the one shown.

    See the 2nd attachment; I re-drew the schematic using Cadsoft's Eagle.

    I added in the mic preamp, revised your LED output drivers to be a bit less confusing and to work more reliably, and added a cap to block DC current from passing through the speaker, which could damage both the speaker and your PIC.

    Changing from using all interconnecting wires for power/ground to symbols gives you a lot more freedom to move portions of the schematic around, and also helps remove "clutter" so that you can quickly see the important signal paths.

    Also, try to keep from crossing over wires as much as possible. I still have a couple of wires crossing, but it's quite minimal.
    I used Vdd and Vss instead of Vcc and GND because for one thing, the datasheet uses Vdd instead of Vcc, and for another, those are the designations used in the default libraries for the PICs. Using the library pin names avoids the problem of having the board "air wires" being connected improperly.
    Last edited: Sep 8, 2011
    fran1942 likes this.