First Schematic - Feedback?

There are three things wrong (that I can see right away).

1) The SER input should be connected to ground (never leave inputs on CMOS chips floating).

2) The 8 inputs need resistors to pull them down to ground, (100k would do) otherwise they will stay charged up to a high level for an indeterminate amount of time after you release the button.

3) There should be a small ceramic capacitor (100nF is OK) from VCC to gound close to the chip.

Michael Kellett

Am 15.02.2012 06:23, schrieb Thomas Sloan:

Hello All,

       Hopefully this is the right forum for this. I just made my first schematic of and was looking to see if anyone had suggestions, corrections, etc. they would like to offer? I'm kinda new to all this (been programming on a Netduino for a while now, and gernal programming for years) and was thinking for my first project I would make a breakout board for a 8-Bit Parallel-In/Serial-Out Shift Register - 74HC165N,65274HC165N,652 from Sparkfun.com. I'm hoping to make the board and use it in a DIY Guitar Rig Controller. Anyway, I was just hoping to post a picture of my schematic and see if anyone saw any mistakes that a newbie like me might make. Any suggestions are welcome. Thanks!

 

PS>>  "Pin_13", "Pin_12"&  "Pin_10" refer to the pins on a Netduino the IC pins connect to

 

>

  Image:SR_Breakout.png

 

>

Your pic din't make it to the newsgroup but I saw it on element 14.

The 165 has no power supply. The 165's inputs are floating (hanging in

the air) until a button is pushed. You need pull down resistors

additional to each input line.

--

Mit freundlichen Grüßen / With best regards

Joern Paschedag

On 15/02/2012 05:23, Thomas Sloan wrote:

Hello All, Hopefully this is the right forum for this. I just made my

first schematic of and was looking to see if anyone had suggestions,

Welcome,

I'd like to echo other comments, particularly Michael's, but with a

little more explanation.

SER should indeed be connected to either ground or VCC.  Even if you're

only intending to read eight bits at a time (before re-loading the

internal register from the A-H inputs) and won't read as far as the SER

input, unconnected ('floating') logic inputs consume unspecified amounts

of current and may result in generally odd behaviour propagating through

the shift register.

Each input A-H should be pulled to ground with a large resistor.  If a

switch is open the corresponding input is left to float.  Depending on

the characteristics of the input circuitry in the 74165, an input might

get stuck 'HIGH' after its switch is disconnected.  This stuck condition

may be permanent or may resolve back to 'LOW' after some charge

dissipates.  Or you may end up with weirdness in between.

100nF capacitors across chips' supplies, placed physically close to each

chip, are always a good idea.  Google 'decoupling capacitor'.

The supply pins for the 74165 aren't shown.  If these hidden supply pins

to the 74165 are named VCC and GND (as they are in the standard

libraries) then EAGLE will implicitly connect them to nets of the same

name.  This will work for VCC but your ground net is called GND(T), so

the 74165's ground connection will not be automatically made.  You may

instead wish to use the 'GND' symbol from the supp1.lbr library.

There are arguments for and against allowing EAGLE to do make implicit

VCC and GND connections.  I prefer to avoid it because it adds

ambiguity, particularly if you are working with many different supply

voltages.  Instead, use the INVOKE command to obtain the second part of

the 74165 device (The 'PWRN' gate), then connect those power pins to VCC

and GND.  This also gives you a good place to add a decoupling capacitor

to your schematic.

Finally, just a stylistic point -- please keep supply components

conventionally oriented.  The ground symbol should point downwards and

the VCC symbol should point upwards.

Other than that -- looks fine

Andrew

0xADF

First off, thank you all for your responses. They are all helpful and have taught me some things I obvisouly did not know

I've made the corrections suggested above. I'm not sure I got the capacitor connected right, but I think I get the whole concept of "Decoupling Cap" now (draw voltage from the charged capaciter giving the power supply time to adjust for the fluction in power consumption). I did also get two new error now when I wired up the SER pin and INH pin to GND. The errors are the same which is "Only INPUT pins on GND". I think this may be something to do with EAGLE more then a error in my Schematic (from what I have been reading), but by all means please let me know if I'm mistaken. Again, thank you so much for all you help. I'm sure I'll be back with more questions!

Hello Thomas,

Your capacitor is Ok but the resistors are not right !

The problem is that input pins on a logic chip must always be at a well defined high or low state and never open circuit. When your switches are closed the IC input will be pulled high through the 100k resistor. This is OK but the resistor makes things (like noise sensitivity) worse. When the switch is open the IC input is open and this means that it's logic state is undefined.

Our suggestion was that the switches are connected directly to the IC as you originally had them but that the resistors go, one from each IC input pin, down to ground, so that when the switches are closed the inputs are connected directly to VCC and when the switches are open the IC inputs are pulled down to ground via the resistors.

Michael Kellett

Hi,

Firstly, +1 for Michael's advice about pull-down resistors, more info

here: http://en.wikipedia.org/wiki/Pull-up_resistor

The errors are the same which is "Only INPUT pins on GND". I

think this may be something to do with EAGLE more then a error in my

Schematic

Ah.  Now that you have the 74165's power pins on the schematic, EAGLE no

longer automatically connects them to GND and VCC, because it assumes

you've INVOKEd them to connect them to something yourself (perhaps to

connect VCC to +3V3 or something).

You will need add VCC and GND connections to these pins.  EAGLE is,

quite rightly, warning you that the only pins currently connected to GND

are 'input' pins whereas it's normal to have at least one 'supply' pin

on this net.

EAGLE's electrical rules checker uses pin-specific information (set when

designing a schematic symbol) to decide whether the circuit makes sense

electrically.  If, for example, you connected QH and !QH together an

Electrical Rules Check would warn you that two output pins are trying to

drive the same net.

Andrew

0xADF

a liitle bit OT, but have a look at:

http://www.williamson-labs.com/

section Bypassing

r

Yikes! I can't believe I totally missed the part about pulling down the pins to GND. With the Netduino, the pins have built in pull-up resistors so you could directly connect a switch to a GND pin and a input port without issue (assuming you enabled the pull-up resistor in your InterruptPort constructor). Anyways, ver3 of my shcematic (and by the way, in case you were wondering, here is the Fritzing diagram I was using as a point of refrence for building this: http://netmftoolbox.codeplex.com/wikipage?title=Toolbox.NETMF.Hardware.InputPortShift).

1) Added pull-down resistors to pull the IC pins to GND when the switch is open

2) INVOKED the GND and VCC pins on the IC and wired each to +3.3 and GND respecfully (Power will be comming from a Netduino at 3.3V)

3) Added a decoupling capacitor connecting pins 8 and 16 on the IC (GND and VCC).

Hello Thomas,

I think you are OK now.

MK

What are you trying to do with this?