Review of First PCB Layout

Status
Not open for further replies.
G

groover

Junior Member level 1
Joined
Oct 9, 2014
Messages
19
Helped
0
Reputation
0
Reaction score
0
Trophy points
1
Visit site
Activity points
172
I wonder if someone would be so kind as to review my first attempt at a PCB? It would be very much appreciated.

Thanks! Groover

Warning! Huge 15 MB "intelligent" schematic file.
 

Attachments

  • PCB1-TopCopper.pdf
    44.6 KB · Views: 136
  • PCB1-BottomCopper.pdf
    19.6 KB · Views: 117
  • PCB1-Schematic.pdf
    14.7 MB · Views: 159
Last edited by a moderator:

I haven't seen much critical signals here.....Crystal circuitry is routed OK. 50 Mhz Controller with Rise and fall times of 3ns ..for most of the outputs you have resistors which will still decrease the rise/fall times. I am not sure about CAN Bus....... I didn't see much problems for this.
 

Great big split in bottom copper pour.
GND for the xtal ref caps, its a rather long path around to get GND back to the IC, can you shorten it?

Plenty of acid traps.

Thin tracks exiting connectors - can you thicken them up where they exit the pad?

Your ground could do with several stitching vias.

What software was this done in? It looks like CADSTAR.
 
Thanks for the feedback - very helpful!

I'm not sure how to eliminate the acid traps - caused by the copper pour?

I am using Design Spark.
 

Remove thermal relief from SMD pads, increase pad to copper clearance (it will disappear when etch compensation added at the moment). Remove thermal relief from vias.
I would move J1 j2 if possible further down the board so you can re-route the can etc. and move the bottom copper split further down the board where it is less harmful.
Move R12 nearer the pin it pulls up and join it to VDD with the trace that comes out of R2.
Move U2 down and put C8 at the top so its near the pin it is decoupling.
ETC.
ETC.
 
Thanks - all great advice.

Can you please confirm though - removing the thermal spokes on pads means that the pads merge into the copper pour completely. The soldermask exposes the pad still though.

Is that better than the thermal spokes? Won't I have an issue heating up the solder during reflow on those pads? For example that seems to be the issue discussed in this post: https://www.edaboard.com/threads/38506/#post176556

Thanks!
 
Last edited:

Confirmed.

Yes you may have an issue if the pads are not thermally relieved, it depends upon your assembly dept. Some people claim to have never had thermal balancing problems, some are just unaware of them happening because they did not make them and some don't get them because their assemblers are very good. Some have lots of thermal problems because their assembly is not so good and are still using old methods & equipment etc.

Ask your assemblers what they want\need.

BTW - Hey Groover - well done on searching and finding an old thread.
So many come on and ask the same questions that have previously been discussed without searching.

:thumbsup:
 
Is that better than the thermal spokes? Won't I have an issue heating up the solder during reflow on those pads?
Click to expand...
Hardly during reflow but hand soldering will be more difficult. Thermal relief is however required for through-plated pads.

The "acid traps" come from manually routed wires connecting the pads. The thermal relief algorithm usually doesn't generate it.
 
Never thermal relief SMD pads IF they are being reflowed and haven't done for many years (hand assembly can/may be different, depends on how the soldering is being done, how careful they are).
Why haven't I used thermal relief on SMD pads (it has never been a problem), because reflow should be done correctly these days and that means NO thermal gradients across the board preferably and not across a component. What does this mean, it means the whole assembly including the board and pads is ramped up to the correct soldering temperature following a correct profile, anything less is unacceptable.

PTH pads are a different matter and are generally solder via a wave for single sided placement or by some form of selective soldering when double sided SMD placement is used, here the solder is applied hot to the pad so any heatsinking action caused by planes etc connected to the pad can cause soldering issued, also the volume of solder and getting the solder up the barrel of the hole come into play.
 
An acid trap is any junction where the angle is less than 90 degrees.
This allows acid\etchant to be trapped in the very tip of the angle and "can" remain even after cleaning, over time it "can"\"may" etch the track away.

An old issue, does not happen a lot these days but there is no excuse for not tracking with it in mind.
 
Here is how it looks now.

I decided to stay with the thermal spokes for the pads, but removed them for the stitching vias.

I don't see any easy way of increasing the thickness of tracks entering/leaving pads in my software. I would have to create small track segments and individually manipulate them. The signal tracks are 6 mil.

Thanks.
 

Attachments

  • CANopenBlocks-Digital-TopCopper2.pdf
    47.5 KB · Views: 151
  • CANopenBlocks-Digital-BottomCopper2.pdf
    22.1 KB · Views: 142
  • CANopenBlocks-Digital-Schematic2.pdf
    14.7 MB · Views: 161

The ground pathes for some bypass capacitors are still long, the ground meshing could be improved by moving some traces on the bottom side and placing additional vias.
 
The best I can do is remove the copper pours. Here it is.

Thanks for the suggestion about the grounds on the decoupling caps. I've made some tweaks to hopefully improve that.
 

Attachments

  • CANopenBlocks-Digital-BothCopper.pdf
    38.2 KB · Views: 135
Last edited by a moderator:

Try and reroute your tracks so that you get more unbroken ground on the bottom, concentrate on getting your tracks on the top side sooner so you have a better ground.
Some examples are scribbled in the attached pic (using the snipping tool lol)



You have blue tracks that go right across the entire board splitting the ground in 2 - this is bad.
A little rerouting and you can improve this a lot.

R1 & R13 are quite a distance away from U2's pins.

Mitre the tracks coming out the bottom of the crystal.
Thicken them up coming out of connector pins.
Bring the track from J6 pin 2 over the top and down so that you can then swap the tracks over on pins 4 & 6 and get into the connector without adding vias.
come out of the caps and via down to the bottom ground.
can you move C8 further away from the edge? if its a COG cap it is liable to cracking if a scored board.

J4 pins 7 & 9 have acid traps on that could easily be fixed.
 
Thanks Matty - lots of good suggestions, which I will implement. I'm learning a lot!
 

Status
Not open for further replies.

Similar threads

Menu
Log in
Register
Cookies are required to use this site. You must accept them to continue using the site. Learn more…