Why no vias or traces allowed underneath SMT inductor, inbetween its pads?

Hello,
The Wuerth inductor 7447709330 says in its datasheet that one should not use vias or traces between its pads....

Wuerth 7447709330 inductor Datasheet...
https://www.farnell.com/datasheets/1736312.pdf

Why is this?

Should the same restriction apply to the similar Coilcraft part, ie the MSS1210-333ME..

Coilcraft MSS1210-333ME inductor datasheet
https://www.coilcraft.com/pdfs/MSS1210.pdf

why does the coilcraft datasheet not mention any such via and trace restriction for underneath the body of its inductor like the Wuerth one does?

A shielded inductor should be OK but the general advice is not to pass traces (or vias which imply a trace is there) in close proximity to the magnetic field around the core. It is simply to eliminate the possibility of inductive pick up either from coil to trace or trace to coil.

Brian.

..thanks, so do you think that passing traces under the inductor, but on the opposite side of the pcb is also a bad thing?....also, what if this is a general filter inductor, carrying pretty much pure-ish DC, then surely there wouldn't be a problem then in routing traces underneath this inductor.?..I mean, nobody says we have to use this inductor in a switching power supply.?..if its not used in a switching power supply, does the "no-traces-between-the-pads" rule still apply?

It isn't a rule, only a recommendation so it's really up you to decide whether there is risk of induced voltages or not. In the case of DC I would assess the risk as low although I haven't seen your actual product of course. As to the reverse side of the PCB being safe, again it depends on the strength of field, PCB substrate is virtually invisible to magnetism. Possibly there would be some screening if the PCB had internal copper planes. Bear in mind that although the inductor may be carrying 'almost DC', there will be a kick of induced voltage if the DC is turned on and off and depending on what the trace connects to, it might cause problems.

From a mechanical point of view, check the screening on the inductor doesn't sit flat to the PCB surface or you could cause a direct short.

Brian.

It is a general guidance for a good design in terms of EMI, avoiding it as much as possible, anyway depending on specific electric environment of the application we can bypass the recomendation, just taking the care to do not route any track the same direction along the magnetic field.

I do not believe it is an EMI issue, rather one of solderability with a large mass sitting on 2 tiny pads. The solder mask and keepout zone is designed to yield the best surface tension for self alignment during reflow.

tiny low mass SMD's can tombstone with the wrong pads and flux, but large SMD's can get misaligned or have bridged gap and result in excess/insufficient solder when masked by hot tracks between pads. So pad size, solder mask and reflow profile is critical for,high yields.

Thus consult with your Assembly shop for DFM rules on this part. Glue dots might help if tracks are unavoidable between pads, which is an extra process cost.

Thanks, the underside of the 7447709330 inductor is slightly unusual.....there is the pads, and then inside the pads, there is a kind of raised bit of metal which appears to be covered in insulating conformal coating, and is in the space between the pads, and is connected to them...you can see the shaded bit of the picture in the top left of the 7447709330 datasheet....I wonder if they fear track shorting to this metal bit?.......however, its unlikely because any tracks between the pads would be covered in solder resist and also the metal bit itself is covered in conformal coating, and appears to be raised into the body of the inductor so that it is held up above the PCB between the pads...of course, vias often have no solder resist over tham, so they would just be relying on the con coat of the underside of the inductor and the fact that the metal bit is raied off the pcb.

Its interesting, certainly no other SMT inductor datasheet says you cant route tracks or vias between its pads.

its very inconvenient, I need thermal copper pour between the pads, thermally relieved to the pads with thick reliefs for good thermal transfer, I also need thermal vias to bottom thermal copper, so not being able to put vias between the inductor's pads is very inconvenient.

Being on the receiving end of EMC & manufacturing failures can also be inconvenient.

thanks, yes but having a small track covered in solder resist is unlikely to skew the inductor on its pads surely?....and as for EMC, I wont be running any digital signals under that inductor, (in fact I wont have tracks at all under the inductor , just vias) I just need to put thermal vias there down to bottom layer thermal copper....so surely there is no emc problem?

no EMI issue

just soldering issues if near tracks between pads for insufficient solder / heat under large thermal,shadow

contact sources for better explanation if you like.

At DC no, but if an inductor was being used in say a SMPSU then there are lots of switching currents around the inductor & diode, hence a general rule of thumb to not route underneath them.
The other side of a ground plane maybe, but even then is it wise to put a plane underneath them too?

In your case maybe the running of a track underneath may not induce any EMI, so its possibly OK - this is why we have "rules of thumb" and we break those rules depending on the thumb in question

Skewing components can happen, usually only if they are small - large items like inductors are not likely to. If it has any form of connectivity to the terminations underneath then I would not run a track under there in case any oles in the mask allow a short to the track. However, as above - rules are meant to be broken & if it's your only choice then go for it.

Without doubting the considerations about avoiding magnetical crosstalk, the context of the keep-out area specifications quoted in post #1 clearly refers to possible solder problems, or more exactly avoiding shorts with the metal sheets at the inductor's bottom side.

If crosstalk (or eddy current) related, the data sheet would require a cut-out through all layers. But it only refers to component side copper features.

The PD series inductors (and many similar types) have an air gap with respective stray field towards the PCB, and it's in fact suggested to avoid it's vicinity with sensitive signal traces. For a trace through the inductor axis, the induced voltages cancel out, however. But there's capacitive coupling as well.

The original question shows that footprint specifications are arbitrary to a certain extent. Obviously both inductors have quite similar design, and many other manufacturers are providing the same industry-standard form factor. So the keep-out area doesn't seem to be absolutely necessary. It might be the case, that Wuerth fears protruding metal edges of the bottom pins, potentially hurting the solder mask underneath the part. And other manufacturers don't.

Thanks, we at first prefer the wuerth inductor because the metal bit underneath it appears to offer greater heatsinking to the inductor, but as you describe, there is the possibility of it shorting to vias underneath it, and so that does indeed look like the reason for prescribing a track and via keepout area between its pads, and that is the reason that we will neglect the Wuerth part and use the coilcraft inductor instead...because we need thermal vias beneath the inductor.

Most inductors have larger metallic pads than the land pad on the pcb, so it is advisable to avoid vias and tracks under the inductor in order to not get shorts.
It would be better to check whether Coilcraft does not have similar issue but simply they do not mention that in their datasheet, leaveing the decision to the layouter.

Most inductors have larger metallic pads than the land pad on the pcb

Click to expand...

...Sorry I do not understand why this would be wanted?...if anything, the solder resist outside the pad could hold the inductor pad up off and away from the pcb pad during soldering?.
Not only that but the hot inductor pad could end up melting into the solder resist, preventing the inductor from settling nicely onto the pads.

treez said:

...Sorry I do not understand why this would be wanted?...if anything, the solder resist outside the pad could hold the inductor pad up off and away from the pcb pad during soldering?.
Not only that but the hot inductor pad could end up melting into the solder resist, preventing the inductor from settling nicely onto the pads.

Click to expand...

It is not wanted, this is how the inductors are constucted. And because of that vias and tracks should be avoided under the inductor. On the inner via edges the solder resist is very weak and can easily create shorts to the metallic pad that sits on the via.