Problem on 0402 package

Am 02.08.2010 10:53, schrieb Marco Trapanese:

Hello,

 

the company which mounts my boards complains about EAGLE 0402 package.

They say "the pads are too much large" and a lot of components are lost

during the soldering (reflow) due to the "tombstoning" effect.

 

I'm wondering if anyone ran through this problem, because I'm sure the

EAGLE library is ok.

 

Anyway, I don't know what tell them. In fact, they ask me a charge for

new components and manual soldering (it means it's my mistake).

 

Marco

Hello,

these packages are part of our libraries since several years. We didn't

have complaints

concerning the sizes of them. The packages follow the IPC standards, and

so I think they can't be too wrong.

just my 2cents

--

Mit freundlichen Gruessen / Best regards

Richard Hammerl

CadSoft Support -- hotline@cadsoft.de

FAQ: http://www.cadsoft.de/faq.htm

Il 02/08/2010 14.33, Richard Hammerl ha scritto:

Hello,

>

these packages are part of our libraries since several years. We didn't

have complaints

concerning the sizes of them. The packages follow the IPC standards, and

so I think they can't be too wrong.

I will bet on this. It's just to talk about, because I think my supplier

did something wrong and now it complains for everything...

Marco

They say "the pads are too much large" and a lot of components are lost

Can it be compared to Cream area, like Cream "hole" not same as pad size.

In DRC | Masks | Cream, my Cream settings are 0mil, ie not extra area for

cream

Maybe could be check with gerber viewer or reading gerber files.

Also 0402 can come from different libraries, like rcl, and other libraries.

Is the problem on all 0402 or only some kind of them (resitors only)

If problem is too less solderpaste on board, maybe the boardhouse has

ordered too thin a pastemask for production.

Just my thoughts...

Christen

Il 02/08/2010 15.41, Christen Fihl ha scritto:

Can it be compared to Cream area, like Cream "hole" not same as pad size.

>

In DRC | Masks | Cream, my Cream settings are 0mil, ie not extra area for

cream

Maybe could be check with gerber viewer or reading gerber files.

The same applies here.

Also 0402 can come from different libraries, like rcl, and other libraries.

Is the problem on all 0402 or only some kind of them (resitors only)

For all components (resistors and capacitors).

If problem is too less solderpaste on board, maybe the boardhouse has

ordered too thin a pastemask for production.

If I'm not wrong they told me there was too much solderpaste so the

components moved from their position.

Marco

If I'm not wrong they told me there was too much solderpaste so the

components moved from their position.

What can too much paste do?

1) Spread to other pads?

2) ??

The solder should hold the components in place, if they get into contact

with each others. The surface tension will pull components into center

I have had same problem (tombstone) in my home office (50$ oven in the

garden), as some resistors only soldered on one end, leaving the other end

up in the air.

Here my solder paste might have dried out a bit before mounting components,

so they did not get into contact, or I simply did not press them firmly

enough onto the board (into the solderpaste).

PS: I have not worked with 0402, smallest are 0805, as I do my own

prototypes, and I am getting older...

I would check my pad size, and ask what size the company request. Too-much

is not that precise specification

Marco Trapanese <marcotrapaneseNOSPAM@gmail.com> wrote:

I'm wondering if anyone ran through this problem, because I'm sure the

EAGLE library is ok.

I just recall the 0402 pads were too large for the comoactness U

required, so I did my own. Could it be that they are meant for wave

soldering? Google for tombstoning and you will find out why this happens

on very light components. Pad size and position IS critical.

"Morten Leikvoll" <mleikvol@yahoo.nospam> wrote in message

news:1232800121302465937.313441mleikvol-yahoo.nospam@news.cadsoft.de...

I just recall the 0402 pads were too large for the comoactness U

required, so I did my own. Could it be that they are meant for wave

soldering? Google for tombstoning and you will find out why this happens

on very light components. Pad size and position IS critical.

Sorry for typo. Sloppy Iphone typing... First line should be:

"I just recall the 0402 pads were too large for the compactness I"

Marco Trapanese: worte

Hello,

>

the company which mounts my boards complains about EAGLE 0402 package.

They say "the pads are too much large" and a lot of components are lost

during the soldering (reflow) due to the "tombstoning" effect.

>

I'm wondering if anyone ran through this problem, because I'm sure the

EAGLE library is ok.

>

Anyway, I don't know what tell them. In fact, they ask me a charge for

new components and manual soldering (it means it's my mistake).

>

Marco

>

"Richard Hammerl"  replied

Hello,

>

these packages are part of our libraries since several years. We didn't

have complaints

concerning the sizes of them. The packages follow the IPC standards, and

so I think they can't be too wrong.............

The libraries only control the pad dimensions.

I suspect DRC settings could cause one-off problems with the standard

footprints.

Verify with a gerber viewer what the Board house and assembler see.

SolderStop that is to distant from the pad does not prevent solder from

running away from the pad along the attaching trace, enabling the leverage

for tombstoning.

A Cream setting that covers the entire pad may be to much for the standard

libraries 0402s.

Perhaps the PCB has  a mix of massive componants and 0402s, the Cream

stencil thickness may have been choosen to satisfy massive parts and so

excessive cream is being applied.

Perhaps the positioning file has an offset error that is manifesting itself

when the tiny 0402 are placed (offset so one end of the chip wins the

surface tension tug of war.)

A quick Google found

http://www.xs4all.nl/~tersted/PDF_files/Plexus/tombstoning.pdf

Most of the findings are assembler issues.

Another 2 cents worth

Warren

Morten Leikvoll schrieb:

I just recall the 0402 pads were too large for the comoactness U

required, so I did my own. Could it be that they are meant for wave

soldering? Google for tombstoning and you will find out why this happens

on very light components. Pad size and position IS critical.

Yes. And I remember that in a german mailing list the IPC pad size

suggestions have been discussed contrarily - obviously they tend to be

too large in many cases for whatever reason, even when specified for

reflow soldering.

The probability of tombstoning rises significantly if the pads extent

too much beyond the part - the melting paste pulls the part up. The pads

should be more "under" the part's contact than "besides" it.

Tilmann

Am 03.08.2010 08:24, schrieb Tilmann Reh:

Morten Leikvoll schrieb:

 

>> I just recall the 0402 pads were too large for the comoactness U

>> required, so I did my own. Could it be that they are meant for wave

>> soldering? Google for tombstoning and you will find out why this happens

>> on very light components. Pad size and position IS critical.

 

Yes. And I remember that in a german mailing list the IPC pad size

suggestions have been discussed contrarily - obviously they tend to be

too large in many cases for whatever reason, even when specified for

reflow soldering.

........

As far as I remember there was a change for the 0805 package in the

past. The

reason was that the original pad sizes did not allow to lay, I believe,

a 0.3mm track

between the two SMDs.

--

Mit freundlichen Gruessen / Best regards

Richard Hammerl

CadSoft Support -- hotline@cadsoft.de

FAQ: http://www.cadsoft.de/faq.htm