Printed Circuit Board Assembly & PCB Design SMT Electronics Assembly Manufacturing Forum

Printed Circuit Board Assembly & PCB Design Forum

SMT electronics assembly manufacturing forum.


via under a smd pad ?

Views: 7856

our boards have many smd pads that has vias under them so wh... - Nov 05, 2007 by omid_juve  

#52299

via under a smd pad ? | 5 November, 2007

our boards have many smd pads that has vias under them so when the screen printer wants to print the solder paste on it , it will penetrate through the via to the bottom side of the board and cause many problem for us . i want to know that is it standard in designing the pcbs to use via under the pad ? Thanks

reply »

#52301

via under a smd pad ? | 5 November, 2007

Hi,

We are also interested in this, and I have heard you can get the PCB's with the via's plugged. Also, if the via's are small, the solder should not penetrate?

Anyone have any further info?

Grant

reply »


aj

#52302

via under a smd pad ? | 5 November, 2007

Hi,

We have had this before - yes they can be plugged and metalised on top .

aj...

reply »

#52428

via under a smd pad ? | 9 November, 2007

Of course if you are an OEM you could go back to your design engineers and tell them via's in SMD pads is unacceptable. Put that in your DFM design guidelines.

If you are an EMS provider you can also influence your customer by explaining the impact that has on the manufacturing process and reliability of their product.

Regards, JD

reply »

#52488

via under a smd pad ? | 13 November, 2007

Hi,

What is this unacceptable? Designed the PCB is much easer if this is possible, so it would be really good to know why via in pad is a problem in production.

Grant

reply »


kpm

#52491

via under a smd pad ? | 13 November, 2007

For the simple fact that the via in the middle of the pad causes the solder to wick into the hole instead of flowing out across the pad and part. Thus cause insufficient solder issues.

reply »

#52492

via under a smd pad ? | 13 November, 2007

From a manufacturing standpoint, this isn't very nice. Vias will tend to wick solder away from the pad, resulting in insuficient solder joints, which require touch-up. The amount of times any solder joint is reheated should be minimized, as extra heat on the component or the pads could cause degredation over time, ie. reduced reliability.

Also, as an EMS provider, additional touch up requires additional handling of the boards, which costs more. While this situation is ocasionally necessary to the design, we charge more for processing this type of design.

And, finally, via's in 0402 or smaller pads could end up being larger than the pad itself (I have 3 assemblies in house right now that are like this with 0402's); we've experienced more tombstoning on these parts, which, on top of causing more touch up as above, also leads to more component loss during production.

Cheers ..rob

reply »

#52505

via under a smd pad ? | 13 November, 2007

Hi,

What size via's are you guys seeing, as the ones in our products are incredibly tiny, and via's are very small now days. The via's on the boards we have are dramatically smaller than the pad on an 0402.

Grant

reply »

#52516

via under a smd pad ? | 14 November, 2007

I had one project with micro-vias in 0805 and larger pads, with no issues.

But my most recent project had vias that were larger than the 0402 pads that the via was in. To the point that for a number of the lands, there was no visible pads (a couple of them...you could actually see a sort of outline where the pad would have been, but all of the plating was taken up by the ring of the via).

The determination was that the designer definitely used vias that were too large for the pads that he used them on. I couldn't give you the measurements off hand, but it was definitely a matter of the designer using the wrong size vias for the pads.

cheers ..rob

reply »

#52518

via under a smd pad ? | 14 November, 2007

Hi,

Those via's sure do sound large, and I think the designer must have made a mistake in the PCB design do you think?

From looking at our PCB designs, if we moved to via in pad, it would really reduce the size of the PCB, so this is an important issue for us. This is why if it's done right, and the via is very small, then the issue for me is knowing if anyone else has done this, and it's worked ok. What were the considerations?

Grant

reply »

#52522

via under a smd pad ? | 15 November, 2007

I do think that the designer goofed, and used too large vias. I believe he only used on size via on the entire board, regardless of whether it was in a pad, or out on the board.

I have seen vias in pad work, though. From a manufacturing standpoint, we used a thicker stencil to apply more paste, knowing that the paste was going to wick into the via. What may be needed, in some instances, is a step-down stencil, so that a thicker layer of paste is placed on the pads with the vias, but a thinner layer of paste can be laid down on the fine-pitch devices.

At a rough guess, I wouldn't want to see a via in a pad that's larger than say 30-40% of the pad size.

All said, as with many other things in manufacturing, it is do-able...it's just a matter of the level of pain involved in the doing. We've placed 0402's on vias that are larger than the 0402 pad, and reflowed them...the only trade off was that the units required additional touch-up after automated assembly.

cheers, ..rob

reply »

#52588

via under a smd pad ? | 20 November, 2007

#52594

via under a smd pad ? | 20 November, 2007

In my past experience, having via's under or attached to SMD lands produces risk. Solder will not consistently wick the same if it is being drawn into a via. This has also caused issues from solder wetting through the via to the other side causing a small bump. Which in turn, causes unseated surface mount components on 2nd side placement. I would not want to add any risk by putting via's under SMD's or in SMD lands...especially with the smaller components being used.

reply »

#52614

via under a smd pad ? | 21 November, 2007

From info I have been told from design standpoint, via in pads helps with managing EMC issues with working design, in particular for high speed digital/dense populated type PCB's.

We had a manufacturing customer that had very low yield because of this via in pads was two big and solder was drained away from the pads - 1000s of pads on design - lots of rework.

It can be done but via size has to be as small as possible, or preferably plugged vias used with solder. This all adds on cost to PCB Fabricator and end user, smaller the via harder to make PCB.

If the designer can avoid via in pad , makes manufacturers happier.

Thanks

reply »

#52626

via under a smd pad ? | 23 November, 2007

Question: We have an issue right know on a prototype batch with via in the pad on an very small pcb 50x50mm (in a panel of course). The designer has no room to move the vias as they said. The pcb is to packed with components also 8-layers. It is also a high speed board... what's the standard recommendation, IPC or what ever, if any, for vias in the pad when we are talking about BGA and vias in the pad? Personally, I cant think of any worse situation than this... Or, if it is No, then I would appreciate this info as well, since I will give it to them... Sincerely, Mika

reply »

#52628

via under a smd pad ? | 23 November, 2007

There a several things you can do to prevent the solder wicking down the hole with the current design, and that's where you should focus. Cost goes up as you go down the list, but in neither case do you need to respin the board, have solder starvation, nor need to do more than little to no rework. * Via plug - From opposite of component side, 50~75% of via, nonconductive epoxy. * Via fill - From opposite of component side, +2 mils, -10 mils of conductor surface, nonconductive epoxy. * Via fill and plate over - Conductive or nonconductive epoxy. No via hole in pad for SMT.

Background references are: 1 �Impact of Microvia in Pad Design on Void Formation,� F. Grano, et al, SMTA International Proceedings, September 2003. 2 �Assembly Issues with Microvia Technologies,� L. Harjinder, and S. Sundar, SMTA International Proceedings, September 2003. 3 �The Effect of Via-In-Pad Via-Fill on Solder Joint Void Formation,� A. Singer, et al, IPCWorks Proceedings, October 2003. 4 �BGA Solder Void Correlation to Via-In-Pad, Via Fill, Surface Finish, and Lead-Free Solder - Final Report,� C. Shea, et al, Pan Pacific Microelectronics Symposium Proceedings, January 2007. 5 "Microvia-in-Pad: Possible Outcomes and Solutions" C. Shea, et al; Circuits Assembly 2/07 p44

You might still be able to download #5 above authored by our old buddy Chris Shea. Certainly SMTA members can download #1 & #2.

reply »

#52629

via under a smd pad ? | 23 November, 2007

Thanks a'lot Dave F, We will look into this as soon as possible. You can't imagine of how much I appreciated your replay. Sincerely, Mika Ps. My Swedish > English => Swenglish, is not so good... Ds.

reply »

#52634

via under a smd pad ? | 24 November, 2007

Hi DaveF, I had a short look into the Nr1. IMPACT OF MICROVIA-IN-PAD DESIGN ON VOID FORMATION Most interesting reading, but one thing though, I could not find any information about the oven profile. Just a picture of it. My question is of about the ramp that they show of the solder profile on Figure 5 page 3/9. Nothing is mentioned about the actual solder profile in terms of temp increasing degr/sec in the ramp-up and degr/sec in the cooling zone. Max 2-4 Celcius degr/sec normally, but for such good work as they did, they should at least mention the slope degree... Neither was there any info about the temperatures in the different oven zones.

However, I must say it was interesting and it is possible that I missed this info and it is not that important either. We know what it takes... I still got the "overall picture". /Best Regards

reply »

Plasma Prior to Conformal Coating

Heller Industries Mark 5获得了 2015年中国SMT远见奖 - 回焊炉领域