Symbol drawing for TCS3200

I have drawn a symbol for the color sensor module TCS3200. I’m still not quite an expert on this, can someone tell me if I’ve drawn the symbol correctly? Have I correctly defined the roles of the pins (output/input etc.)?

I am attaching here the role of all the pins:

There are a few thing not correct here.
The most important is that the pin numbering does not match the funcion. Look carefully at the numbers and the names of the pins.

Second thing is to make a distinction between schematic symbols and PCB footprints. Schematic symbols are for Humans. Therefore, group pins by function, try to keep GND on the bottom and the power supply on the top, and in general signals flow from left to right.

The PCB footprint is what you will put on the PCB eventually. These pads on it do not have hames at all, but just the numbers. And the matching is done with the numbers in the schematic symbol. Therefore it is important that the numbers match.

Normally one numbers the pins starting from 1, not 0. It won’t match up with the footprint pad numbers if you don’t start from 1. (Are you a programmer? :wink:) All the select and ~OE pins are Input, only the OUT pin is an Output. Note that ~OE is active low so in the text you ought put a bar over OE with ~{OE}.

Did I correct things correctly?

~OE should be an Input pin.

Yes, I just noticed and corrected it…

You might also want to put all the select pins on the left even if it looks unbalanced because if you draw the signal flow from left to right, it’s more likely those pins will be connected from the left.

I would appreciate it if you could explain to me better what you mean
I understood what you were suggesting to do but I didn’t understand why…

It is easier to understand schematic if all signals at schematic go from left to right (microphone input on the left and than after a pre-amplifier and voltage amplifier and power stage it go out of schematic to the loudspeakers).
When designing symbol you can suppose signals to it will come from left and signals out of it will go to the right.
But it is only the general rule. If you know your symbol will be used in different context than you can do it your way.

I understood, thank you!
Does this look better? :sweat_smile:

I short VCC and GND names to V and G just to help me made the whole symbol as small as possible. I like them being small as I want to have all my schematic being one page and you don’t know how many elements you will have to use.
I also place name and reference out of symbol as in most cases I have them at schematic out of symbols.

Thank you!
Great tips for a beginner like me. :sunglasses:

I am writing from Win7 PC while I have moved with my KiCad files to V6 so I can’t have it here. I took from my schematic pdf one element with its use:

RE,DE,D are inputs.
R is the output but knowing how I will be using it I placed it on the left.
A,B are out of this simple calssification :slight_smile:

1 Like

You may think about splitting the symbol into two units with additional 2 pin power box. This method allows full names for VCC and GND. Rotated V looks like a >. Extra power box improves schematics what becomes important if your design uses more than one IC. All power box may be moved to a corner of the schematic page and have a 100nF capacitor already assigned as a pair to its later position in PCB.

For power symbols I never use VCC nor VC but +3V3 or 5V what provides more usefull information with same space. GND and negative symbols always looks southward while positive power is oriented north.

‘better’ is debatable.
If you power some HC circuits just from microcontroller output pin.
If you use PMOS to power some circuits.

An example.
We have battery powered RFID reader with ZigBee connection to base stage. Task was to consume 0 current while not working. So ater pressing the button everything switches on and at the end microcontroller have to have the way to switch it off.

I used here 100nF for years and it was very big mistake.

Since (about 2006 I think) we moved from Atmega to AtXmega VCC is for me always 3V3 so I have no doubts seeing VCC at my schematic (here it was VCC but I just cut the picture).
I use 2 layer PCBs with whole bottom being GND. Because of this it happens me to use 0R to cross lines. It is better to use one 1206 to jump with VCC over 4 signal lines the 4 0603 to jump with them over VCC. Because of this my VCC sometimes is divided into few nets so I need more symbols for the same VCC. I use: VC1,VC2, VC3 and so on. Using 3V3 will make these symbols more complicated.

Thats why it was already edited this in the meantime to your reply. Beside formal correctness, sketching schematics is artwork what requires skills like painters have for aqaurell or other specialized things. A great video about from our friend @devbisme is here:

Late reading this post…
On the OE\ or ~OE or whatever, I usually use the “inverted” pin for clarity. This pin adds a small bubble near the base of the pin. It just makes it easier for me to instantly notice the pin in a “not” pin.

1 Like

Nice ! I learned something today :smiley: