Problem with resistor network

Schematic
1

Hi, I’m designing a PCB with 2x 4 resistor networks for a shift register. My expectation would be that one of each 4 legs of the chip would go to one end of the resistor network, and 4 buttons (pads in my case) to the other side of the network. This is how it looks in the schematic:
image

However, when I start designing the PCB, the legs are all over the place:

image
image741×629 44.4 KB

I would expect pins 14, 13, 12 and 11 of the chip to connect to pins 1, 2, 3 and 4 of the resistor network respectively, and then pins 5, 6, 7 and 8 to the pads. What am I doing wrong?

3

It’s very clear from your schematic that, for example, pin 14 connects to pin 2

image

if that’s wrong then you should fix your schematic . . .

4

That doesn’t look like the correct footprint for a 4 resistor star network. Usually they have all pins/pads inline, pin/pad 1 being common. What you have looks like 4 separate resistors in one package.

5

I’m using the KiCad default footprint Resistor_SMD:R_Array_Convex_4x0603. Doesn’t feel like this footprint is correct:
image
A resistor network is essentially 4 resistors glued together in parallel (correct me if I’m wrong), so it should be pins 1 to 4 connected together (common) and 5 to 8 be R1, R2, R3 and R4, or viceversa.
I could edit the footprint, but I want to get this manufactured, and I don’t know if that will mess with the manfacturer’s process.

6

Your footprint shows 8 pads. Your symbol shows 5 pins. 5 does not equal 8. You have a problem.

7

But you use symbol for THT resistor network having one common pin.

8

@SrSosio
Kicad does not have default footprints.

Kicad does not have a SMD resistor array footprint with 5 pads. You will need to find an appropriate Data sheet and create your own footprint.

9

No, I’m not. Where do you see the holes in that symbol?

image
image1699×604 57.9 KB

jmk, by default I meant I didn’t download it. It was in KiCad library when I installed it.

10

That is a SMD resistor array without internal connections.

Your symbol shows a resistor array with internal connections.

To use that footprint you need to change your symbol resistor array to one without internal connections.

11

ok, found it, I think I need to use the R_Pack symbol, instead of the R_Network. Thanks jmk, that hinted me in the right direction.

2 Likes
12

If you fetch the datasheet for the footprint that you selected you will see this:

image
image720×160 22.1 KB

The diagram is the second one for MNR14. It’s 4 separate resistors as I said. If you want to use this part then you should use a different symbol and in your case 4 of the pads should be connected together.

The correct order of design is to first choose the part that you intend to use, from datasheets, then to get suitable symbol and footprint for it, not to use KiCad’s library to go shopping.

13

There are a lot of different types of resistor networks. The one you have chosen has a common pin for all the resistors. These can for example be used if you need pullup resistors on a bus. Another type of resistor network is for voltage dividers, these have all the resistors in series (often high accuracy, low drift etc).

From your description it looks like you want the R_Pack04 variant, which has all connections of the resistors separately available:

image
image1041×736 105 KB

KiCad also has a R_Pack4_Split type, in which each resistor of the symbol can be placed separately on the schematic, but they still combine in a single footprint.

14

Symbols are at schematic. Footprints are at PCB.
You are speaking symbol and showing footprint.
In symbol you have one side of all resistors connected together and provides at one pin. Don’t you see it?

Edit.
After answering I read the next posts.