• Welcome to our site! Electro Tech is an online community (with over 170,000 members) who enjoy talking about and building electronic circuits, projects and gadgets. To participate you need to register. Registration is free. Click here to register now.

2 layer pcb layout tips ?

Status
Not open for further replies.

ItsMike

New Member
Hey everyone,

I'm working on my first 2 layer SMD board and I'm looking for tips for layout.

Which layer should I use as a ground plane ?
How should I connect components from the other layer to the ground plane ? just a via ?
Should the other layer be a power plane ?
Should I care about the amount of vias ?
 

ItsMike

New Member
Oops, seems like I forgot to mention I'll be making the board here [LINK].

I'm using eagle, and I have downloaded the DRC file and so far my design (which looks awful btw) doesn't come up with errors.
The pcb prototyping service above mentions "Minimum slot 1mm*1mm" what does that mean ?

Also, does eagle automatically add solder mask ? or do I do it manually ? if so, how ?

EDIT:
I've just finished routing the pcb and I gotta say it's ugly as hell.
I've used vias under IC's and for some reason these damn SMD IC's don't align with the grind very well.
See attached files.
 

Attachments

Last edited:

RCinFLA

Well-Known Member
It is a very good price. It says it includes green solder mask and white parts silk screen.

When using generic file converters, and during board processing, there is always the possible error of mirror imaging. It is always a good idea to include some right reading text somewhere on each layer that would make it obvious if something gets mirror imaged.

You should also try to include some layer alignment markers within the layout.
 
Last edited:

Boncuk

New Member
Hi ItsMike,

your PCB design doesn't look ugly.

Activating layers 29 and 30 you'll see that the solderstop mask is automatically generated.

There are minor "cosmetic" corrections to do, e.g. getting rid of acute angles in traces.

One example: Net N$1 (SCK) is connected to pin7 of the AVR-ISP connector and to the clock inputs of three ICs. There is an acute angle between the AVR-ISP connector and the microcontroller with the trace angling off to the clock inputs of the three ICs.

The connection would be much safer if you don't use a 90 degree angle for that "junction". Better draw two 45 degree angled off traces to join the junction at a cleaner angle.

I don't know the reason why you connected D1 on the top side to the jack. There is plenty of space without collision to route the jack on the solder side for a safe solder connection.

You used a grid size of 10mil, which might cause problems using components with mixed scales (metric and inches). You're better off using a grid size of 0.3175mm (1/80") or 0.15875mm (1/160"). If the latter is being used Eagle will round the grid number to show 0.1588mm, but work with the given parameter internally.

One more hint: Wide screen monitors produce a wide image of the board. Having the board oriented North-South with a small East-West part you have to zoom in and out continuously to get the traces well done. Grouping the entire board and rotating it 90 degrees gives you a better screen display with less zooming work.

Use a grid size of 1mil to get the board on the 0-0 coordinate with the left bottom corner.

Further I do not recommend to create a ground pour with VDD. Use ground fills on both sides to eliminate possible ground loops.

Regards

Boncuk
 
Last edited:

ItsMike

New Member
Thanks a lot Boncuk.

I tried having all my angles at 45 deg, except when switching layers.
These angles are not only cosmetic but also serve a function of having less reflections. I also read that when there is need to connect 3 signals it's best to form a "T" junction for better performance.

I didn't quiet get what you meant with D1 and what is the solder side ? If it's a double layered board doesn't it have solder on both sides ? :eek:
I'll play around with the grid a bit. Maybe i'll get rid of these ugly miss aligned vias.
Too bad I don't have a wide screen monitor, but a great tip nonetheless.

I just wanna make sure, is it ok to place vias like I did ? i.e really close to the IC pins or under the IC it self ect ?

One more thing, if I do a double layer ground pour how should I route the power to the components ? It seems to be a lot messier.
 
Last edited:

ericgibbs

Well-Known Member
Most Helpful Member
Thanks a lot Boncuk.

I tried having all my angles at 45 deg, except when switching layers.
These angles are not only cosmetic but also serve a function of having less reflections. I also read that when there is need to connect 3 signals it's best to form a "T" junction for better performance.

I didn't quiet get what you meant with D1 and what is the solder side ? If it's a double layered board doesn't it have solder on both sides ? :eek:
I'll play around with the grid a bit. Maybe i'll get rid of these ugly miss aligned vias.
Too bad I don't have a wide screen monitor, but a great tip nonetheless.

I just wanna make sure, is it ok to place vias like I did ? i.e really close to the IC pins or under the IC it self ect ?
hi Mike,
While 'T' junctions and 90degree track connections maybe cosmetically ugly, there is NO technical reason against using them when necessary.

When you consider that ALL the mounted components on the copper tracks are soldered at right angles [ 90deg] to the track it self, due to the right angled bend in the component pins/legs.
Where did the 'reflections' at right angled junctions originate from.???

EDIT:
Image extract from a PCB Design Manual. [reference copper track junctions]
It must be confusing to Newbies when laying out PCB artwork, to be told in an opening line in a tutorial document to NEVER do this or that at track junctions and be told a few lines later it causes no performance problems, its purely a subjective cosmetic preference.
 

Attachments

Last edited:

ItsMike

New Member
I've read something about the fact that when you make a right angle the width of the track is 1.41 times wider which changed the Zo of the track and causes mismatched impedance. But it seems that the change isn't even measurable.

Maybe here: http://www.electro-tech-online.com/custompdfs/2011/12/90degbrooks.pdf
And here: http://www.electro-tech-online.com/custompdfs/2011/12/corners-USA.pdf


Anyways, I tried to split up the top pour to both ground and power near the leds, is that wise ?
Now what ? how should I route the rest of the power ?
[See attached file]
 

Attachments

Last edited:

Boncuk

New Member
hi Mike,
While 'T' junctions and 90degree track connections maybe cosmetically ugly, there is NO technical reason against using them when necessary.
A slight objection here, dear Eric: :) Two 45 degree angles offer better mechanical and thermal strenght than one 90 degree angle. I have made it a habit to draw 45 degree connections into every 90 degree junction. 90 degree junctions also bury the possibility of underetching traces within the junction to get the etchant into the small "corner" for a clean PCB. Even my designed PCB of a DDS function generator produces clean triangle and square waves (75MHz) using that kind of "smoothing" traces. The sinus waves are clean and free of artefacts up to 20MHz but will eventually be clean up to 30 - 35MHz after all parasitic capacitances and inductors are balanced.

When you consider that ALL the mounted components on the copper tracks are soldered at right angles [ 90deg] to the track it self, due to the right angled bend in the component pins/legs.
Where did the 'reflections' at right angled junctions originate from.???
Soldering an SMD chip onto a board with angled off traces into the solder pads will certainly take care of shorts if soldered manually. The traces should have a straight connection towards the pads of at least 1.5mm for safety reasons.
EDIT:
Image extract from a PCB Design Manual. [reference copper track junctions]
It must be confusing to Newbies when laying out PCB artwork, to be told in an opening line in a tutorial document to NEVER do this or that at track junctions and be told a few lines later it causes no performance problems, its purely a subjective cosmetic preference.
May be some 45 degree angled junctions are not necessary but the overall artwork just looks neater.

For me it's not only proper function which counts when designing a PCB layout. It's also the beauty of the artwork which counts. (and this is very subjective). :D

Regards

Hans
 

Boncuk

New Member
Hi ItsMike,

D1 is routed on the component side (trace colour red) and could be routed on the bottom (solder side, trace colour blue). Plated through holes will have connections from top to bottom layer, but a small scratch (small drill diameter) might damage the via to an extend that interrupts the pin connection of the jack towards the diode.

A jack is permanently used to insert and remove a plug and mechanical stress on the pins could cause failure.

Here is an example how I connected a 20pin GLCD. Note that almost all traces are located on the bottom (solder side) to occasionally remove the display from the PCB without damage to the through-hole connection.



The vias around the ICs should have a clearance off the SMD pads of about 1.5mm to elinate the danger of shorts when soldering.

Boncuk
 

ericgibbs

Well-Known Member
Most Helpful Member
hi Hans,
I have never heard of mechanical problems due failures at 90deg 'track junctions'.

I have laid out a great number on artworks in my time and also seen many other PCB's with 90deg junctions that show no signs of additional mechanical failure due to being right angled.

Many of the features you keep saying are necessary for reliable operation are not objective, they are purely subjective of the way you prefer to layout your artworks.
I am not saying that you should change the way you layout your PCB's, all I ask, is to point out to the reader, these are your own preferences and they will no way effect the performance of his circuit.

The points I am making are solely related to copper track junctions.

I would totally disagree with 'its the beauty' of the artworks which counts, it the way the circuit performs in service which counts.

I can see no purpose in turning a functional procedure into 'Artform'.

E.
 

Boncuk

New Member
hi Hans,
I have never heard of mechanical problems due failures at 90deg 'track junctions'.
I experienced them when I installed 19" racks in harsh industrial environment. Besides vibrations caused by huge fans the ambient temperature of the switching cabinet never dropped below 80degC during day time, sometimes getting close to 90degC. PCB material (FR-4) can stand pretty high temperatures while copper traces expand and retract regularly with varying temperatures during day and night time. If that happens over an extended time period traces will crack "open" at acute angles.

I have laid out a great number on artworks in my time and also seen many other PCB's with 90deg junctions that show no signs of additional mechanical failure due to being right angled.

Many of the features you keep saying are necessary for reliable operation are not objective, they are purely subjective of the way you prefer to layout your artworks.
I am not saying that you should change the way you layout your PCB's, all I ask, is to point out to the reader, these are your own preferences and they will no way effect the performance of his circuit.
I think pointing out the possible failure of traces is not a matter of personal preferences. If you take a close look at PC mainboards you'll find all kinds of angles in traces, except for one: 90degree angles. I guess the angles are not being used for a better look, but are meant to half stress on traces.

The points I am making are solely related to copper track junctions.

I would totally disagree with 'its the beauty' of the artworks which counts, it the way the circuit performs in service which counts.

I can see no purpose in turning a functional procedure into 'Artform'.

E.
You must have overlooked that I wrote: besides a proper function of the entire circuit the board should look beautiful. (with the latter being my very personal point of view)

Boncuk
 
Last edited:

ericgibbs

Well-Known Member
Most Helpful Member
hi,
Can you please post a link to any formal documented evidence showing mechanical failures on PCB's due to 90deg angled 'copper track junctions'.?


EDIT:
I have searched the web for any reports of failures or problems relating to copper track junctions caused by 90deg intersections.

All I have seen so far are some subjective 'theories' about possible 'signal reflections'. [I assume this could be a problem if the PCB was designed for UHF].
As you know on most PCB's we have to frequently to 'waist' down a track to pass between two pads, this is also a change in impedance of the track.

All the track to pad/doughnut points are in effect 90deg junctions, as are all the on board component soldered pins, also PTH [plated thru holes].

For the users of 90deg track junctions they report no known problems.

E
 
Last edited:
Status
Not open for further replies.

Latest threads

EE World Online Articles

Loading
Top