Pad types/sizes and single sided pcbs and decoupling questions

[eo1668]

Hi,

1) I have this single layer pcb with two right angle 2mm pitch connector. I have create the pad size with round pad and pad size 20 mils larger than the drill size. During pilot run, the production discovered that after few time plugging in/out the wire harness, the solder joint start to crack and the connector become lose.
I have use this part lib for multiple layer pcb and don't seems to have this problem.
Is there any differrence in terms of pad design for single layer pcb and multiple layer pcb?
I was asked to change the pad to oval and enlarge the pad area as much as possible, is there any guide to this?

2) I have this 4-layer pcb, some of decoupling caps are placed at the bottom side of the IC close to the respective vcc/gnd pins. I have some disaggrement with the EMC testing guy in regards to the vcc/gnd via to the gnd and power plane.
He insist that I should lay the pcb such that the vcc/gnd pin from IC pins should go through via to the bottom side decoupling cap. This via should not go the gnd/power plane instead should pull out another trace from the decoupling cap through a new via and than to the vcc/gnd plane. Any one can share your experiences in regards to this?

Thanks in advance for all help.

Best regards,
Pl

[randychase]

Originally posted by eo1668
Is there any differrence in terms of pad design for single layer pcb and multiple layer pcb?


Yes. With a single layer pcb, you have less copper area to adhere to the board material, plus you lose the strength of the plated thru hole tying the two opposite pads together. In general design practice, a single sided board should use a lot larger pads.

We don't address this really with the pcbstandard's libraries (except for the surface mount SMM parts). For example, with a standard 2+ layer pcb, I would easily use a the following padstacks for a 1/4watt thru-hole resistor:

.060" or 1.5mm pads and .035" or .9mm drills.

With a single sided board, I would try to use .100" or 2.5mm pads and .045" or 1.2mm holes.

You can use the same size holes for single sided boards, but it's common practice to use slightly larger holes for ease of assmbly, specially if it's automated.

As far as your specific part, I would add as much copper as I can within reason. This means to use rectangular or oval shaped pads. You may also want to consider using teardrops. I have been known to throw down extra copper on all the pads just for strength.

[randychase]

Originally posted by eo1668

2) I have this 4-layer pcb, some of decoupling caps are placed at the bottom side of the IC close to the respective vcc/gnd pins. I have some disaggrement with the EMC testing guy in regards to the vcc/gnd via to the gnd and power plane.
He insist that I should lay the pcb such that the vcc/gnd pin from IC pins should go through via to the bottom side decoupling cap. This via should not go the gnd/power plane instead should pull out another trace from the decoupling cap through a new via and than to the vcc/gnd plane. Any one can share your experiences in regards to this?


There is a lot of info about this, and it's not all in agreement.

But I would agree with your EMC guy for the most part.

Method in order of noise suppression effectiveness:

1. Tie the VCC/GND pins on the IC to the planes. Tie the caps to the same plane. Try to keep the caps close to the VCC/GND pins.

2: Run the VCC to the decoupling cap and then have the cap tie into the plane. Tie both the IC and the Caps GND to the plane.

3. Run the IC's VCC and GND traces to the decoupling cap. Run traces from the cap to the respective planes.


We have been reviewing some information about things like this and we will be creating some online tutorials and information databases about things like this, and we will include a section specifically on noise immunity techniques, EMC/EMI suppression, grounding techniques, and more.

[Carl_at_xrite]

In all the years I have done decoupling caps place the cap as close to the VCC pin as possible run from vcc to cap then from cap to plane.

When the device operates it changes the impedance seen on the supply line and the capacitor offsets this dip in the supply voltage due to its storage properties.

Just my 2 cents ...

As for Pad sizes on single sided boards, I worked as a designer for AC/DC switchmode power supplies (standard- mass produced in china )
All of the boards were done on CEM3 single sided material.
The smallest hole we could do was .035 with a .080" pad.
this material was hard tooled and punched not drilled so the pad areas had to be large as well as teardropped and extended wherever possible.