I am designing single side pcb board in eagle as hobbyist. I have one schematic diagram. I am trying to make single sided pcb for it as hobbyist



I have placed all the component's but I don't think I am placing at correct position Any suggestion will appreciated

 

Why single sided. The cost is the same as 2 sided.
Why the pin out. Micro to JP2. It looks clean on the schematic but very hard on the board. There are traces that need to cross many places. Can you change the schematic so the layout is clean and the schematic looks like crossed.

 

Also you can see that the port is designated with consecutive port pins, try to mach these up with the header
In this case, probably moving the JP2 header vertically to where D1 is etc. making a cleaner 'ratsnest' visually.
IOW move components to find the cleanest most efficient positions.
e.g. C5 could be rotated 180° ?

 

When designing a PCB, component placement is critical.

1. Think of the flow of signal and power traces. Minimize the length of all traces. Minimize crossed traces.
2. Think of interconnects in and out of the board, i.e. pad placement.
3. Think of serviceability, the ability to replace components.
4. Think of heat flow for high power components.
5. Think of component dimensions, lead spacing.
6. Do not forget mounting holes.

C3 is decoupling capacitor across the 3-terminal regulator.
You still need a similar decoupling capacitor across VDD and VSS of IC1.

Consider standard thru-hole components vs SMD. Why have a mix?

 

Why single sided. The cost is the same as 2 sided.

I am just practicing so no issue with single side

Can you change the schematic so the layout is clean and the schematic looks like crossed.

as per your suggestion I modified design but still don't know how to keep all components on pcb

 

The advantage of a double-sided board is you use the reverse side as primarily a ground plane. This removes heaps of 'GND' wiring from the front of the board, cleans up signals and generally makes things work better. And there's no cost disadvantage.

still don't know how to keep all components on pcb

Can you explain further?

In fact, a lot of my recent boards have been 4-layer with the added avantage of simplifying power connections - the cost differential is rapidly disappearing with automated production by the likes of jlcpcb and ChinaPcbOne .

 

I am totally agree with you Mrchips I can design circuit but I get very frustrated when I try to keep the components on the board. I don't understand how do you know which component should be placed on which position. I think it can be understood only by practicing more

Practice helps. Try to place components to follow the flow of the circuit. Start with inputs to left, outputs to right then play with orientation to minimise crossovers and complex routing. Sometimes it just works, other times you have to try different layouts until one gels.

Its an art-form to some extent...

 

Also, if you have decoupling capacitors these should go right next to the chip and the Vcc trace should hit the capacitor before it hits the chip pin

Here's a simple example from another thread on PCB layout - the top board started out single sided, went double-sided because couldn't make it work without lots of jumpers, decoupling caps nowhere near the device so essentially useless. The bottom, relaid out, double-sided with ground plane, decoupling effective since no need to route ground wires. And see how its simplified the routing.

 

I think it can be understood only by practicing more

You are correct, only practice will improve your skills. If you really are serious, I suggest that you forget about the automatic tools for a while and try doing it manually for a few simple circuits. Use the circiut diagram as reference and draw the components in a similar arrangement. Then try to connect the different nodes together. You will have to shuffle components around a bit to get everything connected with the minimum of jumpers.

I have been designing and building my own printed circuit boards for over 50 years. There were no computer aided design programs back in the 70s. Originally I had to do it manually, on squared paper, with a pencil and eraser but there are lots of easy to use vector graphics drawing tools available now. It is a challenging game of strategy but well worth the effort. I still design my circuits manually. I find that the automatic tools can't design with minimum size as a priority.

Don't give up. It gets easier every time!

Just to inspire you, here are a couple of circuits I designed using Visio (an older graphics tool from the MS Office Suite).

 

Thank you all for your good advices. Now I have come with better circuit than before. In the circuit there is 8051 and power supply circuit. I am not sure layout math with circuit diagram

Please review layout




Layout Image with components

 

Sorry but that's not good. Your Vss trace to the MCU should be thick and short, as should your Vcc, which is missing. Power traces have significant spikey current through them so a long thin run like that will be and inductor and will cause all sorts of issues...

Here's a partial version of a better single-sided layout, all tracks on back of board. Viewing from top through board. Despite being only single-sided there's a substantial ground plane.

 

Here's a partial version of a better single-sided layout, all tracks on back of board. Viewing from top through board. Despite being only single-sided there's a substantial ground plane.

@Irving you have design a very nice and clean layout. your layout is millions time better than my.

I know its time consuming but if you have no problem then Can you design layout without substantial ground plane? its only request because I want to see how do you lay down all components without substantial ground plane?

 

Why do you not like the ground plane?
If you do not like it then replace it with a fat trace.

 

@Irving you have design a very nice and clean layout. your layout is millions time better than my.

I know its time consuming but if you have no problem then Can you design layout without substantial ground plane? its only request because I want to see how do you lay down all components without substantial ground plane?

Of course you can do it without the ground plane, there's just no benefit in not doing so, and modern PCB layout software will put the ground plane in for you, avoiding the existing tracks...

Here's the version without the ground plane, just direct connections (I've also put in the reset button as well)




And here's the version with a complete ground plane, done by just drawing the outline of the board and using the software to flood fill the zone - see how it automatically excludes everything that's not GND, and includes everything that is GND. This is how I would do it for real, its a no-brainer.

 

There are a number of advantages to using a ground plane.
And if you are doing the etching yourself it substantially saves enchant.

 

On the point of "time consuming", you need to get to understand your software and what it can do. For example, all those pin headers and tracks? The footprint is for an 8 x 1 header, so all 8 pins are drawn as one component by the software, as are the tracks (using copy/duplicate) and then all 4 ports are drawn using copy/duplicate & mirror where needed. Total time < 10mins... The total time to lay that out? About 20 minutes total.

Another advantage of using a ground plane is that all the ground connections on parts can be ignored and the software will connect them up for you after you've laid everything else out. Its rare the software can't find a way to every GND connection and its a lot easier that way.

 

With regard to ground planes: have a look at Rick Hartley

He is an absolute Titan in the PCB design field currently. In this video he explains how to design modern high speed boards.

 

here are a couple of circuits I designed using Visio (an older graphics tool from the MS Office Suite)

What template did you use (not that I'd use Visio for that)? I have an old version from 1996 (pre-dates Microsoft's acquisition of Visio) that now runs on Win10.

 

It’s much like untangling a ball of string. Move the components around to straighten the ratsnest.
If you have ICs with two or more circuits (dual op-amps, quad nand-gates), the gates can be interchanged to get the best layout.
Don’t regard the schematic as “fixed”, go back and change it if it improves the layout, for instance, if you have a resistor and a capacitor in series, and they would fit better the other way round, swap them.
Never use a thin track for a power supply connection.
And use the groundplane! Not only does it simplify layout, it makes your circuit work better.
If your board has mains on it, the there are standards you must legally follow.

 

if you have decoupling capacitors these should go right next to the chip and the Vcc trace should hit the capacitor before it hits the chip pin

Good idea.
If you have surface mount capacitors, the Vcc trace should go in one side of the pad and out the other.
That way there's no sneak path for the noise around the capacitor.
Ideally the ground side of the cap would then go directly to a ground plane or ground flood.