Can someone please tell me what I need to add (if anything) to connect this CD4070 IC to this power circuit?
For example, I know that for the TL072 and 74’s that I need to add in two 100n caps. Do I need to add anything like that to the 4070 IC or can I just connect it like this?
I can not find anything about that in the datasheet, but I think it’s good practice to add a 100nF cap between VCC (12V) and ground. I think it’s standard with all CMOS chips as well.
Also note that VSS should go to ground and not -12V, the chip can only handle 15V and between +12V and -12V are 24V already! 
Yes, that’s it.
and… we need 20 characters…
Great! Thank you both for your help!
And be careful to protect it’s inputs from negative voltages.
Just the same as for arduino, you’ll find plenty of schematics, but basically it’s just a resistor and a diode.
Isn’t that what the 5819 diode is for? Or do I need to add in a 10r resistor in addition to the diode?
I am basically taking a schematic and redrawing it in kicad so I can get some boards printed. The original schematic didn’t have the power section split out and for me it makes more sense to split out the power section. I also didn’t see that the original schematic had any 100n caps on the power pins for the ICs so I added those in plus the diodes and elec. caps. Here’s the original schematic that I am working from:
@eric meant protecting the input pins against negative voltages, which is a separate issue from the 1N5819 for protecting the power pins against reversal. But in this schematic the input pins aren’t connected to any input jacks, just to +12 V via switches, so no such protection is needed.
Thanks for the clarification @analogoutput .
@analogoutput , @eric , @sebastian - As I was going through double-checking my schematic for errors I realized that I didn’t have the power for the DG419DY IC in the power section. It looks like in my reference schematic that pin 5 is connected to pin 4 and that goes to +12V and pin 7 goes to -12V and pin 3 to GND. I added this into my schematic but I have a couple of questions.
Looks good to me! Again I did not see any caps in the data sheets, but I would simply add them , they can’t hurt , I guess 
One between +12V and ground and one between -12V and ground, same as opamps would be my suggestion.
If I were drawing this schematic I’d do the TL07x power pins as you have, and omit them from the op amp symbols on the main part of the diagram; they clutter things up without adding information (IMHO).
And I’d do the 4070 likewise. I just noticed power pins are shown on one of the 4070 symbols in the main part. I’ve never seen logic chip power drawn that way, but I guess it’s okay. I’d rather put it in the power section though.
But those are all multi-section parts. For the DG417 which is an 8 pin package with only a single section, I’d leave it out of the power section and just draw it in the main part as it is, and add the bypass cap in the main part.
It’s a matter of taste, but I use the power section only for connections and bypass caps for multi section parts. (Actually I just realized I have a recent schematic with a TL071 where the power is shown in the main part but the bypass caps are shown in the power section. Which makes sense to me given the KiCad TL071 symbol doesn’t have a separate section for the power pins. I guess I could draw my own symbol with main and power sections, but I haven’t.)
100 nF footprints are tiny and the capacitors cost nothing, so adding footprints close to all power pins is a good idea; you can always leave things out when building, and add capacitors later if things behave weirdly.
Also note that you should always decouple from supply rail to ground, so ICs powered with dual ±12 V need two caps each.
Thanks everyone for the information. This is how I have it now. Does this now look right?
On another project I had asked about swapping a 2N3904 with a MMBT3904. I had asked if I should follow the pin numbers on the schematic symbol in KiCad or follow the visual pin outs. Someone said that KiCad should change the pins to their correct numbers, but I found that it didn’t automatically do it. I needed to swap out a BC245A on this schematic as well. The schematic author said to go with a J111 or J112 so I chose a J112 since I have some in SMD. Should I still be following the visual symbol layout and not the pin numbers printed on the symbol like how I have done it below? I am asking again because the project that I had asked my other question on isn’t working and I was wondering if that could be why. Disn’t want to make a similar mistake.
Hi there, just have a look at the datasheet of your specific transistor and find out where G, S and D are located. The pins of an SMD transistor always have the same pin numbers, as shown in my picture.
In the schematic edit the properties of the transistor (upper left window), select the footprint-library (red arrow), and check if the pins of the footprint match the pins and functions of your transistor, if not swap them in the footprint.
I hope this helps.
The KiCad Transistor_FET symbol library has a symbol for MMBFJ112.
It shows the gate as pin 3. The footprint it uses is Package_TO_SOT_SMD:SOT-23:
Pin 3 is the single one, which is indeed the gate on an MMBFJ112, per the datasheet:
So use KiCad’s MMBFJ112 symbol and you should be all set.
The previous talk r.e protecting the inputs, I did not see any mention of the comparator U1B on the Gate-in input, If the gate signal is less than 2v the output of that op amp will be approaching the negative supply rail and connected to an input of the 4070. Having a quick look at the TI datasheet the maximum negative input is -0.5v. I would consider placing a signal diode at pin 7 of the TL074, R11 should act as a pulldown resistor then limiting the input to the 4070 to range 0V - +12v ish.
If I am mistaken, I hope someone corrects me.
Okay great. I used that MMBFJ112 symbol in the schematic. I saw that on the BF425A ( which is the part that I am replacing) that the gate on that one is pin 1. So, you’re right, that will work. Thanks for confirming it for me.
I’m making sure that I understood correctly what you were saying. Did I add in the 100n caps correctly where I needed them? Does the rest of this power circuit look right to you? This is how I have it setup as of now. Thanks for looking
I have just noticed you have moved the +12v and -12v symbols in the schematic to now be before the diodes, in an earlier iteration these were to the right. In the current format, only the power to the IC’s is polarity protected, not the remainder of the circuit.
