Take a look this simple PCB design in PADS

[Md Mubdiul Hasan]

Hello there,

I want to caught those eyes who knows PADS pcb design well.

I wanted to make a very basic OR-gate here.

Take a look the schematic and layout and feel free to critique /discuss/advice me about, 

 

1. Via patterns.

2. layer definition

3. Routing

4. Add drafting

5. Mounting  hole.

6. pour manager

[Md Mubdiul Hasan]

People will give you more feedback if you post images of the board rather than zip files.

Yes, reasonable idea.

Take a look the image now.
Put your advice here.

[DrGeoff]

Why the massive transistors for a couple of LEDs? You could use SMD or TO-92 devices.
I don't see anywhere for power to enter your board.
There's a common connector for the switches but it does not go anywhere (touch pads maybe)?
When laying out a 2-layer board, stick with a convention with top traces in one direction and bottom traces in the other.
Then you are less likely to corner yourself. Do the power rails first, and add a power decoupling cap near the logic device (since we do not know anything about the power supply to the board).
Unterminated inputs on the logic device should be avoided.

[Md Mubdiul Hasan]

Thank you sir Geoff,
Take a look my feedback

Why the massive transistors for a couple of LEDs? You could use SMD or TO-92 devices.

Yes, well noticed the fact. I dont have any SMD type transistor decal.
Can you give it to me ? What I have is attached.
Yes, we can also make it our own.

I don't see anywhere for power to enter your board.
There's a common connector for the switches but it does not go anywhere (touch pads maybe)?

Can I use a 2 pin connector here for power? What about SIP-2P decal?

When laying out a 2-layer board, stick with a convention with top traces in one direction and bottom traces in the other.

Dont you mean in layer defination , TOP and BOT can be set to Horizontal and vertical?

Then you are less likely to corner yourself. Do the power rails first, and add a power decoupling cap near the logic device (since we do not know anything about the power supply to the board).
Unterminated inputs on the logic device should be avoided.

If I add a connector this problem will not be solved ?
Lets assume decoupling capacitor stay at external PS.

[DrGeoff]

Thank you sir Geoff,
Take a look my feedback

Why the massive transistors for a couple of LEDs? You could use SMD or TO-92 devices.

Yes, well noticed the fact. I dont have any SMD type transistor decal.
Can you give it to me ? What I have is attached.
Yes, we can also make it our own.

I don't see anywhere for power to enter your board.
There's a common connector for the switches but it does not go anywhere (touch pads maybe)?

Can I use a 2 pin connector here for power? What about SIP-2P decal?

Yes, that would work fine. Hopefully you can sort out what your switches are supposed to be doing.

When laying out a 2-layer board, stick with a convention with top traces in one direction and bottom traces in the other.

Dont you mean in layer defination , TOP and BOT can be set to Horizontal and vertical?

No, I mean when routing. I assume you routed this simple board manually. It would be crazy to use an autorouter on it.

Then you are less likely to corner yourself. Do the power rails first, and add a power decoupling cap near the logic device (since we do not know anything about the power supply to the board).
Unterminated inputs on the logic device should be avoided.

If I add a connector this problem will not be solved ?

No. You need to terminate the unused logic input correctly.

Lets assume decoupling capacitor stay at external PS.

Let's not. That defeats the purpose of decoupling caps.

[Md Mubdiul Hasan]

Isn't the common pin (pin 2) of the switches supposed to be connected to VCC?

Thank you blueskull.

Dont you mean switches and U1 not powered correctly?
Do you think switches need a power path with capacitor each ?

[Md Mubdiul Hasan]

Yes, that would work fine. Hopefully you can sort out what your switches are supposed to be doing.

Does it means it needs a pull-up power with suitable capacitor ?
The main IC has not been powered well, did you see?
I got this circuit from a TEXT book.

No, I mean when routing. I assume you routed this simple board manually. It would be crazy to use an autorouter on it.

No I did manually.

No. You need to terminate the unused logic input correctly.

Can you draw here, little bit.

Let's not. That defeats the purpose of decoupling caps.

Dont you mean a coupling capacitor should be add from the SIP-2P connector positive pin to ground ?

[Md Mubdiul Hasan]

Stop building things and go to read some books. If you happen to be in a university, go to ask professors.
You need a LOT of things to learn.

I do agree, but I wanted help for pcb also, at this point, I did not consider the circuit logic.

First, where is power input? Where do you plan to bring your 5V and GND into the system?
Second, as I said before, if you want to set logic input level high when button is pressed, you need to tie the switch to VCC, so as the user presses the button, it conducts electricity and sets logic level high. When use releases button, the pull down resistor sets logic input lo

My posted circuit is more symbolic, how to think about this circuit in attachment ?

In a no ground plane design, run a thick wire beneath the chip from GND to VCC, and connect to the VCC capacitor.

Which tools you usually use for pcb design ? I am considering a GND plane, that is 1 among 4 layer.

[Md Mubdiul Hasan]

Well, for the case of denouncing your idea is good, but putting a capacitor across a switch is also convenient.
The denouncing theory is   nicely presented here, http://www.ganssle.com/debouncing-pt2.htm

[bson]

I took a quick stab at it, and apart from your bullseye SPST pads I don't see a hard need for vias other than to connect to a solid bottom ground plane.  (The switches will need a pull up, and 33ohm is too big for a pull down, but maybe I misread the tiny print.)  The component designators don't match yours, but I just wanted to demonstrate it's pretty easy to route this.  I didn't have bullseye pads on hand (and wouldn't personally use them anyway).





To note on your layout, it looks like the diode silkscreen orientation is the reverse of the A/K pins.

You can swap units in the 'LS32 to use different pins.

You can replace the transistors with a different jellybean device in TO-92 or whatever  that works as well for switching but have a more convenient EBC pinout, if that helps.  Or a dual device in a small SOT package.

You don't have power supply pins (I added those or it wouldn't ERC/DRC).

[bson]

Or, somewhat quickly again, diodes neatly placed side by side, switches ordered, Vcc pullup on the switches.  Again, just to give you ideas on how to think about layouts...  You can move the Vcc pin, or use a 2-pin power connector, or rearrange things quite freely without it getting complicated.  The first step though is to simply start by thinking of the bottom copper as a ground plane, then ignore ground while straightening out the rat's nest.  Then if you have a few crossed lines left see if you can find different parts, packages, or swap units (or I/O pins on microcontrollers).  It can usually be straightened out, mostly.

[Md Mubdiul Hasan]

I took a quick stab at it, and apart from your bullseye SPST pads I don't see a hard need for vias other than to connect to a solid bottom ground plane.  (The switches will need a pull up, and 33ohm is too big for a pull down, but maybe I misread the tiny print.)  The component designators don't match yours, but I just wanted to demonstrate it's pretty easy to route this.  I didn't have bullseye pads on hand (and wouldn't personally use them anyway).





To note on your layout, it looks like the diode silkscreen orientation is the reverse of the A/K pins.

You can swap units in the 'LS32 to use different pins.

You can replace the transistors with a different jellybean device in TO-92 or whatever  that works as well for switching but have a more convenient EBC pinout, if that helps.  Or a dual device in a small SOT package.

You don't have power supply pins (I added those or it wouldn't ERC/DRC).

Great effort!
But which design tool you have used?

[Md Mubdiul Hasan]

I took a quick stab at it, and apart from your bullseye SPST pads I don't see a hard need for vias other than to connect to a solid bottom ground plane.

I understand, how many planes did you used?  I have use VIA for complicated path way in circuit.

(The switches will need a pull up, and 33ohm is too big for a pull down, but maybe I misread the tiny print.)  The component designators don't match yours, but I just wanted to demonstrate it's pretty easy to route this.  I didn't have bullseye pads on hand (and wouldn't personally use them anyway).

This switch need to have power and de-bounce RC combination, see the comments put in above.

To note on your layout, it looks like the diode silkscreen orientation is the reverse of the A/K pins

.
Lets see again that mistake.

You can swap units in the 'LS32 to use different pins.

PADS design give you all necessary setting in "attributes"
 

You can replace the transistors with a different jellybean device in TO-92 or whatever  that works as well for switching but have a more convenient EBC pinout, if that helps.  Or a dual device in a small SOT package.

Yes, I have 3 pins SMD, need to edit in layout.

You don't have power supply pins (I added those or it wouldn't ERC/DRC).

Yes, I will use 2 pin.


Great effort!
But which design tool you have used?
[/quote]

[David Chamberlain]

Hi Md Mubdiul Hasan

I think you mentioned your focus was more on the PCB layout but I think you need to pay more attention to the schematic / electronic design side of things first, otherwise what's the point?

The inputs to your OR gates only have a reference to ground and themselves so pushing those buttons would seem to do nothing?

I googled this for you.
https://circuitdigest.com/electronic-circuits/or-gate-circuit

The example in the link shows how you could achieve the same thing without discrete transistors at all.

If you post for help it would be really nice, and this goes for all in general, if you could provide some context around the motivation and background. Is this a school logic assignment or are you really just trying to learn PADS / PCB layout only?

If its the PCB alone then I have a few thoughts...



1. Just neaten this up a little.. the one to the left of it looks good.
2.  Just swap these LED's and you've saved yourself a jumper trace, in fact I think this whole board could be done on one layer.
3. unless you've placed that component on the bottom side of the board its not going to connect to any copper.
4. Why does this via poke out like that.
5. also if you go this way you don't need it anyway.

[edit] single layer if you select a different button type.

David

[bson]

But which design tool you have used?

I used a fairly recently nightly OS X build of KiCAD...
http://kicad.info/

[Md Mubdiul Hasan]

Dear Sir David Chamberlain,

Thank you for nice feedback. This is what I wanted to know !

My intention is to make the pcb good looking, matched with relevant design rules, small scaled and can be manufacture.
I know this simple design can made in single layer, but I want to work out other layer also.

Take a look the modified design here.
I have added the connector, de-bounce capacitors, resistors.
Feel free to criticize.

[n1ist]

Just looking at the last PCB:
- I don't see a ground pour connecting all the pads highlighted in white
- The current=limiting resistor to the top LED is miswired.  It should go between VCC and the LEDs
- The LEDs are backwards
- I would use a wider trace for VCC to reduce impedance
- The decoupling cap should be right next to pin 14 of the IC
- Unused inputs of the IC should not be floating
- The button pads are shorted by the topside trace between the center pad and ring
- Just to verify that you will be using either snapdisks or carbon-backed buttons; otherwise the footprints aren't right
- I haven't looked at the schematic but the network on each button looks wrong - a cap in parallel will tend to pit the contacts, and why have the voltage divider?
- The via size looks very small
- You have silk screen on the pads - either it won't get printed since many board houses use the mask layer to keep the silk off the pads, or if it is printed, it will float off the pads during soldering and make a mess
- There are no mounting holes
- I would add to the silk
  * voltage and polarity on the power connector
  * board name and rev
  * your name and possibly email


/mike