Evaluation of pcb board routing

Thread Starter

Glebiys

Joined Mar 11, 2019
16
Hi!

I'm creating a PCB on which the ESP32-DevKitC V4 module will be mounted. From it will move the connectors. I ask you to evaluate the layout of the board, I will be glad to criticism.

Thank you!

Top:


Bottom:
 

MisterBill2

Joined Jan 23, 2018
5,785
Without checking that all the connections are right it looks OK. The minimum-etch style does work well most of the time. I do see one place where the common connection is floating, which is towards the bottom left corner of the upper image. It is not totally isolated but only one skinny strip connects it.
 

jpanhalt

Joined Jan 18, 2008
9,094
Looks OK to me too. Nice job for #1. Some designers make the ground pad a different shape (e.g., square) on multi-pin, through-hole devices. That's a bit helpful, say, for a single row header. You might also consider making your silk screen font a little larger or heavier font. Don't be stingy with it. It is free.
 

eetech00

Joined Jun 8, 2013
1,868
Hi

You might want to re-check the copper track, pad and pour clearance requirements.
There are a lot of locations on the board where the pour did not fill past pads and tracks.
The board fabrication house usually provides their capabilities....which might affect the various copper clearance settings of your board design.

I noticed that the silkscreen outline of the IC body seems to touch the copper pads. You might want to check that the silkscreen doesn't touch the copper pads...there should be a clearance setting for this in your PCB Design software.

one last thing...
Before sending to board fab house, review the gerber files with a gerber viewer.
Doing so can be quite telling...I use "DFM Now"...its free.

eT
 
Last edited:

MisterBill2

Joined Jan 23, 2018
5,785
If the silkscreen had component numbers and pin numbers it would be a lot simpler to comment on possible changes, such as one that might avoid two PTHs and a spacing issue. Also, one side should be marked "top". Boards with no markings are perceived as not being worth repairing, not the impression that you want to give.
 

Thread Starter

Glebiys

Joined Mar 11, 2019
16
Thanks for the help! I tried to make all the corrections. Modified version (font is enlarged, connectors are displaced, dimensions of tracks and vias are enlarged, cleaned up blank areas).

Top:


Bottom:
 

eetech00

Joined Jun 8, 2013
1,868
Thanks for the help! I tried to make all the corrections. Modified version (font is enlarged, connectors are displaced, dimensions of tracks and vias are enlarged, cleaned up blank areas).

Top:


Bottom:
hi
Don't mean to be picky...but you asked:)
This is a pretty simple board but I still see a lot of unfilled copper pour areas.
The copper pour should easily fill all areas of the board.
For example, the pads for the ESP32 pins should be surrounded by the copper pour.
Either the clearance is too wide, or the pad size is too large, or both.
A little hard to tell, but it seems like the trace widths could be narrower. The pour should also pass between the IC pins..

Just to give you an idea of the required trace width. Below is a screen capture of the gerber viewer while querying one of the traces on the ESP32 artwork. Its using 8 mil traces.

ESP32sample.png

Also,
Should the mounting holes isolate the mounting screws from the ground plane?
The ones shown do not. Something to check....

eT
 
Last edited:
The connectors don't have a pin 1 marked. The ESP32 doesn;t have pin 1 marked. It could even be a square corner on the rectangle.

the connector silk screens makes it easy to be able to insert the connectors 180 degrees. There are likely features on the connector.
 

MisterBill2

Joined Jan 23, 2018
5,785
The connectors don't have a pin 1 marked. The ESP32 doesn;t have pin 1 marked. It could even be a square corner on the rectangle.

the connector silk screens makes it easy to be able to insert the connectors 180 degrees. There are likely features on the connector.
Isolated copper pours may tend to couple circuits that may not benefit from capacitive coupling. In fact, I am wondering about the benefit of copper pour, if there is any benefit at all. It does add weight and value, so it may not be beneficial.
Certainly adequate marking of all connector orientations is useful if any part is hand-built, but less useful if the process is 100% machine stuffed and it is never intended to be repaired.
 

MrSoftware

Joined Oct 29, 2013
1,742
It's a good idea to add your own model number and revision in the silk screen. It might not seem important now, but a few months from now, or after you've made a couple of revisions (sometimes unexpected) it makes it a lot easier to know what you have in your hand. It also makes it easier when you you're debugging a physical board and need to refer back to the schematic. Knowing the revision of the physical PCB will tell you which schematic revision you need to look at.

Also you'll want some indicators showing which hole is pin 1, usually a dot. And on your LEDs you probably want something in the silk showing the orientation. On the power connectors it can be helpful if the holes are marked + and -, and if there's room you can even put the voltage. That can be helpful should you need to debug it at some point.

Overall nice job for a first board!
 

eetech00

Joined Jun 8, 2013
1,868
Isolated copper pours may tend to couple circuits that may not benefit from capacitive coupling. In fact, I am wondering about the benefit of copper pour, if there is any benefit at all. It does add weight and value, so it may not be beneficial.
Hi

The ESP32 has noise generating circuits...WiFi, 200Mhz+ clock, etc., so there may be some benefit...
If interested, here is an article from Altium on 2 layer PCB ground planes.

https://resources.altium.com/pcb-design-blog/understanding-ground-planes-in-your-two-layer-pcb

eT
 

Hemi

Joined Mar 17, 2012
12
Just a few more suggestions.

- make the vias larger that are connecting the traces on the top to the bottom. Your PCB fab probably has limits on their size and it's better to go larger especially if drill registration is off a little bit.

- place a large copper pour under the 3.3V LDO tab to provide some heatsinking to that component. Depending on how high your VIN is, even go as far as to place a polygon on backside of the board as well and stitching them together with vias to help pull heat from that component. I also prefer to stitch the top and bottom ground planes together around the vreg especially in the situation you have where there's only a couple small traces connecting ground to the rest of the board.

- I don't see any reverse input protection. If your connections are polarized, not as much of an issue but since you haven't labeled what each pin on any of those connectors does, will you remember which is + and - a year from now? I always label each pin on a connector so there is no guessing what each pin is for. Like someone else said, if you're going to pay for the silkscreen (or it's free), use it as much as you can. If silk screen isn't free, then use the stop mask to label things.

- speaking of silkscreen, beef up the line widths. What you're using looks smaller than 5mil and won't be very legible.
 

SLK001

Joined Nov 29, 2011
1,543
I do see one place where the common connection is floating, which is towards the bottom left corner of the upper image. It is not totally isolated but only one skinny strip connects it.
+1 on this observation.

Also, you don't need to use thermal relieved ground pads anywhere on this board (I don't use them ANYWHERE on ANY board). You should also add many ground vias to stitch top and bottom grounds together as one. Also, modify your PIN 1 on all your parts so that you can identify them on the copper. If your field pins are circular, then use a square pad for PIN 1. Circular pads are a little more difficult to solder by hand, so I would use oblong pads (make PIN 1 of these rectangular shaped).

I would have a mounting hole on all four corners, not just two. It greatly increases your mounting options.

You will need to modify your silkscreens so that they fit on areas where there is mask. A lot of times, a vendor will not place cutaway any screening where no mask exists. Place your part numbers OUTSIDE the screen area where the part will go so that it can be read once the part is on the board.
 

MrChips

Joined Oct 2, 2009
20,888
MrSoftware made a good point about adding Model Number/Revision/Date in the silkscreen.

When I used to make my own double sided PCB it was important to add text on top copper layer so that you can instantly see that you have the top-bottom orientation correct while setting up the photo masks.
 

bug13

Joined Feb 13, 2012
1,832
Here are my personal preferences:
  • use a good ground plane, the ground should be as solid as possible, ground should be bottom layer (unless you are doing RF)
  • use a VCC layer, this should be top layer, route all your signals on this layer, all SMT should be on this layer
  • all SMT components should be on top layer if possible, GND should be via to the bottom layer immediately
  • maybe the input the output filter caps can be close to the voltage regulator
  • have a ground pour on top layer around the voltage regulator and stitch the round together with lots of via as heat-sinking (as already mentioned)
  • solder mask tenting for all your vias, top and bottom
  • more bigger designators, they all should be the same orientation
  • add a PCB fiducial, if you want it look more professional (you don't need it tho)
  • maybe add some good old 1n or 10n between VCC and GND on all your connectors, if they are going to be long wires.
  • add some cool image you like as skills screen, I usually an add Iron man helmet like this one :)
 

Tonyr1084

Joined Sep 24, 2015
4,379
I like everything pointed out so far. Especially agree with square pads (or rectangular) for pin 1 of all components with polarity. One thing I noticed that I'm not sure of what is going in the 40 pin rectangular pattern is if this is going to be an IC, you have components underneath. I'm hoping you have a plug-in display that goes over it. But if something permanent is going to be soldered in place then you have heat generating components under an IC. Again, I don't know what's going in that space. My first thoughts on the PCB was silkscreen is too small AND there is no pin 1 identifier. Someone mentioned a silkscreen dot over pin 1, that works too. OR an IC illustrated with the pin 1 designator. As I read on I saw the comment about revisions - an excellent idea. I've seen boards designed by experts go through several revisions before settling on a final option. If you have Rev. B (for instance) and Rev C incorporates a new trace, and you have a Rev B board in hand without the new trace it's easy to cut traces and hand wire in new traces, thus, you can upgrade a revision that way.
 
Top