Via size problem with a Ground wire-Resolved(I restarted from scratch)

[MuxDemux]

I'm Currently working on a custom PCB in Easyeda, and after auto routing and cleaning it up a bit I still have one ratline from a capacitor to a pin that is a GND wire. due to the proximity of other pins I had to make a blind via to the wire on inner1 that has a outside diameter of .288mm and and inside diameter of .144mm. I have looked online for if that size is to low and if it that will just break it. It seems that It might be fine because the device is low current, But I was just wondering if this via could work or if their is another solution. I have attached an image of the via and wire. Also the pins directly above and below the GND pin are not connected to anything.

[u666sa]

Electrically, for a low‑current GND connection, your via is fine. Manufacturing‑wise, it’s very likely below their standard capability unless you’re explicitly paying for HDI/microvias.

Change Drill 0.2mm
Pad 0.35 – 0.4mm

[temperance]

outside diameter of .288mm and and inside diameter of .144mm.

If you are pointing at the via underneath the package, how can this via have a drill diameter of 0.144 if the hole diameter seems to almost match the SMD pad size?

Which component is this? More than one vias underneath the package is probably required for proper grounding.

[Psi]

Not to mention heatsinking.
Usually when an IC has pads under it like that is also for getting rid of lots of heat to the gnd plane.

Yeah, we need to know what the component is.

[MuxDemux]

Sorry I did not mention the component. Its the DA14531 by renesas electronics. Its really small, also the package type is QFN. For the Hole size, the clearance set for each pad only allows a hole that wide to fit on the pad or else it breaks the DRC rules. I don't think a via here will work anymore but the space between the inner and outer pads, although not visible is not enough for a wire. also I am talking about the blind/buried via underneath the pad.

[langwadt]

afaict pin 23 is also ground ..

[MuxDemux]

This wire goes to a decoupling capacitor of 100nF before connecting to the larger GND network.

[langwadt]

This wire goes to a decoupling capacitor of 100nF before connecting to the larger GND network.

decoupling ground?

[MuxDemux]

Oops, I seem to have accidently placed it their, Ill just connect the wire into pin 20. Thanks for the catch

[ejeffrey]

It looks like pins 19-21 and 23 are all various ground pins and can just be connected together?  But you have a ground trace going from pins 19-21 through the analog ground pin on the outer ring?  And for some reason wan't a separate trace for pin 23?

That doesn't really seem ideal.  It might not matter for such a low power chip but it adds significant ground inductance.  Is there an app note or reference design you are working from?

Normally i would expect to see a ground plane on layer 2 and all 5 ground pins connected to it with microvias.  You might use one microvia for all 4 central pins, possibly under pin 20 and a separate via for the analog ground.  For a via under pin 20 you can use a bigger annular ring without risking shorting to adjacent pins.  You do need to consider

If you can't use a ground plane, i would still prefer to connect all 4 inner ground pins together if possible. 

[pcprogrammer]

First of all, I would worry more about the crappy routing job done by the auto router.

You mentioned EasyEDA, and I myself would not trust the auto router of it to do a proper job. What I do trust is the DRC checking, which verifies the schematic net list against the routing. This is very nice to have and use, because it assures a proper match between the two.

You might want to post your schematic here too, to have it checked on other issues that might be in there.

If you plan on using JLCPCB for making the PCB, I ran into via size issues too, and asked about what the smallest size is without increasing the price. See the attached table. I mostly work in mils when designing a PCB and have 18 / 10 mil as smallest via size. Normally the via size is 24 / 12.

It looks like pins 19-21 and 23 are all various ground pins and can just be connected together?  But you have a ground trace going from pins 19-21 through the analog ground pin on the outer ring?

The datasheet shows the pins 2, 19, 20, 21 and 23 as noisy grounds, so to me it looks like these can be tied together without problems. Using a proper ground plane underneath sounds like a good idea though, but care has to be taken with the antenna signal and ground. Pin 1 and 18. I'm no expert in this field, but if it was me designing this, I would study how to layout something like this and not use an auto router, and make sure to get the HF part right.

[langwadt]

compared to the example schematic in the datasheet lots of the connections makes no sense

[temperance]

Just some advice for the DA14531. Buy a ready made module.

From the routing shown, it is obvious you will not be able to do this part properly. (The chip requires a lot more vias in the right places to function properly.)

https://www.renesas.com/en/document/dst/da14531-module-datasheet?r=1601921

[MuxDemux]

Hi Thanks for the advice, I linked the schematic here and I think I certainly made some mistakes. I am specifically trying to use the DA14531 to just take the accelerometer data from the BMA530 and transfer it via bluetooth to a separate device. I anyone here see's any kind of mistakes I can fix that would be great.

[pcprogrammer]

When you ask for a review of a schematic or PCB better make sure it is readable. I'm not talking about the PDF being corrupt, I'm talking about the bad practice in the schematic that makes it hard to follow the design.

One plus is that you used wires to make the connections, and not labels, but with the wires running through components and texts it is hard to follow.

A mistake that stands out is the to small capacitance value for the regulator decoupling. These should be 1uF instead of 100nF.

Attached is an example of a more properly drawn schematic. Also see this site for more on this: https://www.reddit.com/r/AskElectronics/wiki/design/#wiki_schematic_diagram_guidelines

[langwadt]

Hi Thanks for the advice, I linked the schematic here and I think I certainly made some mistakes. I am specifically trying to use the DA14531 to just take the accelerometer data from the BMA530 and transfer it via bluetooth to a separate device. I anyone here see's any kind of mistakes I can fix that would be great.

you must be joking, not only is the schematic a mess, all kinds of things are shorted. Start over

[radiolistener]

Just a small note: renaming a thread to "Closed" is not a good practice. People recognize and find topics by their original titles, and changing it to a generic label makes it difficult to understand what the discussion was about. It also comes across as a bit of clickbait, since the title no longer reflects the content.

It would be better to keep the original title and simply mark the topic as solved or closed.

[pcprogrammer]

And to be honest, the topic is far from closed or solved. Both the schematic and the PCB are far from being useful to anyone.

Don't see it as criticism, but see it as an opportunity to learn. Why else would you go to an EE forum and ask for a review?

[SteveThackery]

And to be honest, the topic is far from closed or solved. Both the schematic and the PCB are far from being useful to anyone.

Don't see it as criticism, but see it as an opportunity to learn. Why else would you go to an EE forum and ask for a review?

I think the OP is feeling a bit embarrassed. Of course, titling the thread "Closed" doesn't make it so. 😁

[Psi]

There's nothing to be embarrassed about, every single engineer here went through the same thing and made the same mistakes when learning.