Hi there. I'm having some issues with the routing done in Eagle on my pcb. I'm building a VU meter with an LM3915 and LM3916 based on the schematic here. Attached are jpeg's of both the schematic I've made and the resulting PCB, and the original Eagle files. When I'm looking at the PCB, it doesn't have the +12V and -12V separated. There's only +12V. What have I done wrong? The only differences in my schematic and the one I'm copying is that I've used screw terminals instead of just leaving a hole in the pcb to solder a wire to. What do I need to do to make sure that I have both +12V and -12V, as per the original schematic I'm copying? Thanks for all your help!

 

Well, you connected what should be -12v to +12v, so Eagle thinks that they are the same. Look to the right of C3; there is a junction that connects the wire from POWER pin 3 to the wire from POWER pin 2. The power pins on IC1A are not presently shown in the schematic.

First, go to the board and use the ripup router to remove all of the existing traces.

Next, go to the schematic and delete the wire that is running through the middle of IC1A.

If you don't want to have to add the power pins to the TL072, then skip the next paragraph and use V+, V- and GND symbols as mentioned in the next one to label the respective wires, and Eagle will automatically connect them. If you want to use +12v and -12v symbols instead, follow the instructions in the next paragraph:

Use the INVOKE command (or button, looks like four AND gates in a group on the left toolbar) and click on IC1A. A selection list will pop up, and you'll see "P PWR+- Request" show up. Click on that line to select it, then click OK. You will then be dragging around the power pins (4 and 8) for the TL072. Place them where you had the wire running through the opamp before, and then connect the desired wires (+12v, -12v)to the pins.

You should use symbols from the supply-2.lbr and connect them to the wires so that the schematic power rails are not ambiguous. Use V+, V- and GND symbols, like this:

You could use +12 and -12, but then Eagle would give warnings in ERC about wrong signals being connected to power pins. Warnings are frequently OK, but you want to keep that list as short as possible.

Use ERC early, and often. If you have ERRORS in ERC, you must fix them or the PCB will never be right.

Once you create the board, use DRC to check if you've done anything horribly wrong. Drill sizes are not consistent in some of the libraries; some have holes smaller than 32 mils (0.032"), which Eagle doesn't like. You'll have a hard time plugging a DIP IC into holes that are smaller than 32 mils.

 

Wow, how did I miss that? Is this correct now?

 

Yep that looks right to me. Maybe just approve all those "no value" warnings.

 

That gnd is for shield?

 

That gnd is for shield?

Actually, I think I did something wrong. The original schematic that I'm copying has the two grounds (speaker and power) connected. Will this matter in the circuit? I don't believe it should but I want to make sure before I order a pcb.

 

I don´t really think it matters.

 

I don´t really think it matters.

Ok. Is there any benefit, though? To my knowledge, ideally one connects all the grounds together eventually to prevent voltage differences in the grounds. It's a very simple connection to make in the circuit.

 

I don´t know what you are powering ti with, but in the end all the grounds need to connect together. The third pin is just stays there and nothing needs to be connected to it.

 

I don´t know what you are powering ti with, but in the end all the grounds need to connect together. The third pin is just stays there and nothing needs to be connected to it.

I'm not entirely sure yet but likely just a simple dc power supply with 12V rails. So are you saying that something like this wouldn't work?

 

Yes this would work, but you need to add resistor in series with the LEDs according to datasheet. The voltage for the leds should be less than 7 volts.

As for the pcb, you need much wider traces, also I don´t understand why are led14 and 15 connected the way thay are.

 

LED 14 and 15 are connected that way because I just did it with the Eagle autorouter. it's more simple now that I'm using two layers. As for trace, what width would you recommend? And the resistor would only need to go between the power input and the led's right? I'll be using 3.5V 20mA LED's, so that would mean I'd need a 425ohm resistor, correct? (V=IR, [(12V-3.5V)/.02]=425ohm). Would I just place this between the power input and LED 1?

 

Dang, Wookie.....yer awesome.
LOL!!!!!

 

So here's what I've got now.

I'll be using this center tap transformer and this filter to drop it down to DC +/-12V. It'll be hooked up like this:

CT Transformer > Filter > VU Meter

However, I'm still wondering why and where I'd need resistors. The original schematic here doesn't have them listed, and nor does the datasheet for the LM3915 (see pages 16 and 17 for similar applications). I know the LED's should only run on ~3V, but it looks like the IC's compensate for this need.

Here is a quote from this article explaining the schematic in more detail:

Both IC LM3915 and LM3916 have a change of the display from a bar graph to a moving dot display by one pin. A single supply as high as 25 V and as low as 3 V can operate the whole display system. To eliminate the need for current limiting resistors, the LED current driver is programmable and regulated. Both ICs contain an accurate ten-step voltage divider and an adjustable voltage reference. Ten individual comparators referenced to the precision divider is being driven by the high impedance input buffer which receives signals from the ground and up to within 1.5 V. although it does not require protection from +35V, the accuracy is normally better than 0.2 dB. Since both ICs are very easy to use, only a single resistor may be added to the ten LEDs for a 1.2 V full scale meter. To program the full scale anywhere from 1.2 V to 12 V in dependent of voltage supply, another resistor is required to be added. A single potentiometer can easily control the brightness of the LED.

Please correct me if I'm wrong, but it seems that the current limiting resistor is only needed if I'm using 1 LM3915, not two or with an LM3916. Also, when I add a 470ohm resistor (the closest 5% resistor), it changes the entire V+ line. Are you saying that I'd need to add an individual resistor for every LED? That seems a bit ridiculous and I know people have made circuits like this without doing that.

 

Do you use it in dot or bar mode? Anyway, in the datasheet you posted, on page 2 it says "VLED must be kept below 7V or dropping resistor should be used to limit IC power dissipation."
So ideally, I would use a 7805 to lower the LED voltage and keep the dissipation away from the IC. (or just lower Iled)

 

Do you use it in dot or bar mode? Anyway, in the datasheet you posted, on page 2 it says "VLED must be kept below 7V or dropping resistor should be used to limit IC power dissipation."
So ideally, I would use a 7805 to lower the LED voltage and keep the dissipation away from the IC. (or just lower Iled)

Mostly in bar but I have that switch to allow me to select which mode I'd like to use.

Is there a reason to use the 7805 instead of a 470ohm Resistor? Seems like the resistor would get it closer to 3.5V, whereas the 7805 will regulate it to 5V, which is still too much for the LED (they run at 3.5V 20mA). Perhaps I just don't understand where to place this and what I'm trying to accomplish by adding one of these pieces. Also, note that that part on page 2 appears to only be for a single chip (pages 16 and 17 make no note of this and allow voltages up to 20V for VLED, or at least from what I can tell). Perhaps they didn't list it since they previously did. I'm not sure. I'd like to make sure, though, before I order a custom pcb.

What I'm worried about adding the resistor or the 7805 is that that changes the entire V+ voltage to 5V (or ~3.5V with the resistor). This means that my voltage rails would be unbalanced, with one at +5V and one at -12V. How do I implement these parts such that only the LED voltage is changed, and not the entire +V line?

 

The outputs of the 3916 are constant current, so the LEDs allways get their current as set by R1 and R2 on page 2, lets say 20mA.

The problem is that if the supply for the LEDs is say 20V, then the IC has to drop about 17V@20mA x 10LEDs. This makes the dissipation in the IC when all LEDs are on 3.5W, which is way too much for the tiny package. With 12V you still get 1.8W. When you drop the LED supply to 5V, you have enough headroom for different kinds of LEDs and varying saturation voltage of the outputs, but minimize the dissipation in the IC. Remember that the power still has to be dissipated somewhere, that is in the 7805.

You could use a resistor too, but the dissipation in it would be quite high, so I think it is easier to get rid of the heat in a heatsinked package rather than free-cooled resistor.

 

The outputs of the 3916 are constant current, so the LEDs allways get their current as set by R1 and R2 on page 2, lets say 20mA.

The problem is that if the supply for the LEDs is say 20V, then the IC has to drop about 17V@20mA x 10LEDs. This makes the dissipation in the IC when all LEDs are on 3.5W, which is way too much for the tiny package. With 12V you still get 1.8W. When you drop the LED supply to 5V, you have enough headroom for different kinds of LEDs and varying saturation voltage of the outputs, but minimize the dissipation in the IC. Remember that the power still has to be dissipated somewhere, that is in the 7805.

You could use a resistor too, but the dissipation in it would be quite high, so I think it is easier to get rid of the heat in a heatsinked package rather than free-cooled resistor.

Ok I understand now. So would something like this work? I had to bypass the LED's to maintain 12V for the IC, but keep the LED's at 5V. Is this correct? I'm mainly concerned about the connection at LED 19 where it is no longer connected to V+.

 

Exactly like that, but add the recommended caps around the 7805, 330nF from input to gnd and 100nF from output to gnd, otherwise you are asking for problems with oscillations of the regulator. The caps should be right next to the regulator.

 

So this should be the final, correct schematic?

Also, I'll be using a small center tap transformer with a filter after it to power this board. Will I be able to run two of these boards with the single transformer and filter (2 channels, 1 board per channel)?