Re: [PEDA] tenting vias

[Bagotronix Tech Support]

> I just looked at this a short while ago. I am also using a 388 1.27mm
PBGA,
> by AMD - ELANSC520. We are intending to tent the Vias as the folks on this
> group suggested. I have noticed your Via pad is smaller than we were asked
> to use by our fab house. We were asked to use 0.71mm pad and 0.3mm hole.

0.3mm ~ 12mil, so your via hole is the same.
0.71mm ~ 28 mil, so your via pad is 3mil wider than mine.

I was just going by National Semiconductor's recommended land patterns for
the parts.  They seem to recommend a 0.64mm (25mil) pad for the solder
balls.  They don't specify how big the via should be, but of course it has
to fit between four pads.  I just figured on using the same size for the via
pad.  Maybe that's not such a good assumption?

For vias, I normally use 32mil pad, 18mil hole, but BGA is pushing me into
new areas...

Best regards,
Ivan Baggett
Bagotronix Inc.
website:  www.bagotronix.com


- Original Message -
From: "Colin Weber" <[EMAIL PROTECTED]>
To: "Protel EDA Forum" <[EMAIL PROTECTED]>
Sent: Thursday, August 23, 2001 5:45 PM
Subject: Re: [PEDA] tenting vias


> Ivan,
>
> I just looked at this a short while ago. I am also using a 388 1.27mm
PBGA,
> by AMD - ELANSC520. We are intending to tent the Vias as the folks on this
> group suggested. I have noticed your Via pad is smaller than we were asked
> to use by our fab house. We were asked to use 0.71mm pad and 0.3mm hole.
>
> If your using the same chip, I'd be interested in how it works out for
you?
>
>
>
> At 02:35 PM 22/08/2001 -0400, you wrote:
> >Hello, all:
> >
> >I am designing a board with a 388 BGA chip.  I have questions about vias:
> >
> >1)  Should I tent the vias under the BGA?
> >2)  If (1) is yes, should I tent other vias on the board?
> >3)  If (1) is yes, what substance/method is used to tent vias?
> >4)  If (1) is yes, what do I tell the PCB fab house to get them to tent
the
> >vias?  Is it as simple as "tent the vias"?
> >5)  If blind vias are used, do they need tenting also?
> >
> >The BGA has a 1.27mm ball grid.  I am considering a 25 mil pad, 12 mil
via,
> >31 mil solder mask opening diameter.  Does this sound good?  If not, what
> >would you recommend?
> >
> >Best regards,
> >Ivan Baggett
> >Bagotronix Inc.
> >website:  www.bagotronix.com
> >
> >
>
>
> Regards,
>
> Colin Weber
>

* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
* To post a message: mailto:[EMAIL PROTECTED]
*
* To leave this list visit:
* http://www.techservinc.com/protelusers/leave.html
*  - or email -
* mailto:[EMAIL PROTECTED]?body=leave%20proteledaforum
*
* Contact the list manager:
* mailto:[EMAIL PROTECTED]
*
* Browse or Search previous postings:
* http://www.mail-archive.com/proteledaforum@techservinc.com
* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *

Re: [PEDA] tenting vias

[John Haddy]

My recent reading has indicated that the trend now is to use
non-solder-mask defined lands for BGAs. There is some evidence
that long term reliability suffers if solder-mask-defined lands
are used, as there is a stress concentration point where the
solder ball meets the edge of the solder mask.

In the interests of stress balancing, I match the land size to
that of the contact point between the solder ball and the BGA.

Failing the availability of that information, the next best
guess is to us a land that's 66% of the ball diameter.

Soldermask should be pulled back to the point that that the
collapsed ball won't be touching the SM (in an ideal world...).
This target is another influence on whether or not to use
dry film resist (its increased thickness compared to liquid
photoimagable mans it has to hav a larger SM to pad clearance).

John Haddy

> -Original Message-
> From: Tim Hutcheson [mailto:[EMAIL PROTECTED]]
> Sent: Friday, 24 August 2001 6:24 AM
> To: Protel EDA Forum
> Subject: Re: [PEDA] tenting vias
>
>
> What about the issue of whether to use a solder mask around the BGA ball
> land patterns?  I though I read somewhere that there are pros and
> cons about
> this as it might cause ball breakdown during placement.  If so, what would
> be the correct SM diameter to use with a 25-mil ball land?
>
> Tim Hutcheson
> Institute for Human and Machine Cognition
> 40 S. Alcaniz St.
> Pensacola, FL.  32503
>

* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
* To post a message: mailto:[EMAIL PROTECTED]
*
* To leave this list visit:
* http://www.techservinc.com/protelusers/leave.html
*  - or email -
* mailto:[EMAIL PROTECTED]?body=leave%20proteledaforum
*
* Contact the list manager:
* mailto:[EMAIL PROTECTED]
*
* Browse or Search previous postings:
* http://www.mail-archive.com/proteledaforum@techservinc.com
* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *

Re: [PEDA] tenting vias

[Colin Weber]

Ivan,

I just looked at this a short while ago. I am also using a 388 1.27mm PBGA,
by AMD - ELANSC520. We are intending to tent the Vias as the folks on this
group suggested. I have noticed your Via pad is smaller than we were asked
to use by our fab house. We were asked to use 0.71mm pad and 0.3mm hole.

If your using the same chip, I'd be interested in how it works out for you?



At 02:35 PM 22/08/2001 -0400, you wrote:
>Hello, all:
>
>I am designing a board with a 388 BGA chip.  I have questions about vias:
>
>1)  Should I tent the vias under the BGA?
>2)  If (1) is yes, should I tent other vias on the board?
>3)  If (1) is yes, what substance/method is used to tent vias?
>4)  If (1) is yes, what do I tell the PCB fab house to get them to tent the
>vias?  Is it as simple as "tent the vias"?
>5)  If blind vias are used, do they need tenting also?
>
>The BGA has a 1.27mm ball grid.  I am considering a 25 mil pad, 12 mil via,
>31 mil solder mask opening diameter.  Does this sound good?  If not, what
>would you recommend?
>
>Best regards,
>Ivan Baggett
>Bagotronix Inc.
>website:  www.bagotronix.com
>
>


Regards,

Colin Weber

* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
* To post a message: mailto:[EMAIL PROTECTED]
*
* To leave this list visit:
* http://www.techservinc.com/protelusers/leave.html
*  - or email -
* mailto:[EMAIL PROTECTED]?body=leave%20proteledaforum
*
* Contact the list manager:
* mailto:[EMAIL PROTECTED]
*
* Browse or Search previous postings:
* http://www.mail-archive.com/proteledaforum@techservinc.com
* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *

Re: [PEDA] tenting vias

[Dwight Harm]

I didn't notice anyone mention one other thing -- you can make tenting the
default by using Tools | Preferences | Defaults, select Via, Edit Values,
and check Tenting.

Dwight.

> -Original Message-
> From: [EMAIL PROTECTED] [mailto:[EMAIL PROTECTED]]
> Sent: Wednesday, August 22, 2001 1:18 PM
>
>
> 4)  If (1) is yes, what do I tell the PCB fab house to get
> them to tent the
> vias?  Is it as simple as "tent the vias"?
>
> You select the vias, and check the box marked tenting in
> their property
> page. The Protel won't remove solder mask in the gerber.
>
> Rob

* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
* To post a message: mailto:[EMAIL PROTECTED]
*
* To leave this list visit:
* http://www.techservinc.com/protelusers/leave.html
*  - or email -
* mailto:[EMAIL PROTECTED]?body=leave%20proteledaforum
*
* Contact the list manager:
* mailto:[EMAIL PROTECTED]
*
* Browse or Search previous postings:
* http://www.mail-archive.com/proteledaforum@techservinc.com
* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *

Re: [PEDA] tenting vias

[Tim Hutcheson]

What about the issue of whether to use a solder mask around the BGA ball
land patterns?  I though I read somewhere that there are pros and cons about
this as it might cause ball breakdown during placement.  If so, what would
be the correct SM diameter to use with a 25-mil ball land?

Tim Hutcheson
Institute for Human and Machine Cognition
40 S. Alcaniz St.
Pensacola, FL.  32503

* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
* To post a message: mailto:[EMAIL PROTECTED]
*
* To leave this list visit:
* http://www.techservinc.com/protelusers/leave.html
*  - or email -
* mailto:[EMAIL PROTECTED]?body=leave%20proteledaforum
*
* Contact the list manager:
* mailto:[EMAIL PROTECTED]
*
* Browse or Search previous postings:
* http://www.mail-archive.com/proteledaforum@techservinc.com
* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *

Re: [PEDA] tenting vias

[Jon Elson]

Waldemar Kulajew wrote:

> Mr. Baggett,
>
> some answers for your questions 3 and 4.
> My experience is either to tent the vias only half or tenting them with
> selkscreen (if this is the right word for the lacquer used to show the
> component-positions).
> 1) The first Idea means to use a soldermask covering the pad but leaving the
> holes open. Because my manufacturer told me not to use completely tented vias
> with HAL-soldering (I am still using HotAirLeveling-process) for the air in the
> via burst open the soldermask.

A solution for this is to tent the via only on the side where it is neede, ie. the
BGA side.

Jon

* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
* To post a message: mailto:[EMAIL PROTECTED]
*
* To leave this list visit:
* http://www.techservinc.com/protelusers/leave.html
*  - or email -
* mailto:[EMAIL PROTECTED]?body=leave%20proteledaforum
*
* Contact the list manager:
* mailto:[EMAIL PROTECTED]
*
* Browse or Search previous postings:
* http://www.mail-archive.com/proteledaforum@techservinc.com
* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *

Re: [PEDA] tenting vias

[Waldemar Kulajew]

Mr. Baggett,

some answers for your questions 3 and 4.
My experience is either to tent the vias only half or tenting them with
selkscreen (if this is the right word for the lacquer used to show the
component-positions).
1) The first Idea means to use a soldermask covering the pad but leaving the
holes open. Because my manufacturer told me not to use completely tented vias
with HAL-soldering (I am still using HotAirLeveling-process) for the air in the
via burst open the soldermask. Protel allows a negative soldermask expansion for
vias (and 99SE allows it layer-specific if you need it)
2) The second Idea is a makeshift. For these process can be done after HAL but
haven´t got the precision, you have to place silkscreenpoints manualy and you
perhaps have problems if a plane surface is needed. On the other hand you can
use the points only where you need it. And you have less problems in
komunikation with your board house.

Hope it helps a little.

Waldemar


Bagotronix Tech Support schrieb:
> 
> Hello, all:
> 
> I am designing a board with a 388 BGA chip.  I have questions about vias:
> 
> 1)  Should I tent the vias under the BGA?
> 2)  If (1) is yes, should I tent other vias on the board?
> 3)  If (1) is yes, what substance/method is used to tent vias?
> 4)  If (1) is yes, what do I tell the PCB fab house to get them to tent the
> vias?  Is it as simple as "tent the vias"?
> 5)  If blind vias are used, do they need tenting also?
> 
> The BGA has a 1.27mm ball grid.  I am considering a 25 mil pad, 12 mil via,
> 31 mil solder mask opening diameter.  Does this sound good?  If not, what
> would you recommend?
> 
 - - snip - -

* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
* To post a message: mailto:[EMAIL PROTECTED]
*
* To leave this list visit:
* http://www.techservinc.com/protelusers/leave.html
*  - or email -
* mailto:[EMAIL PROTECTED]?body=leave%20proteledaforum
*
* Contact the list manager:
* mailto:[EMAIL PROTECTED]
*
* Browse or Search previous postings:
* http://www.mail-archive.com/proteledaforum@techservinc.com
* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *

Re: [PEDA] tenting vias

[John Haddy]

I can only comment on what I do (with microBGAs: 0.8mm pitch).

I tent everything that's not used as a testpoint. Most particularly,
at the pitch of BGA I'm using, all vias under the BGA are tented.

With the fine pitch BGA, an untented via results in a soldermask
opening that intersects with that of the adjacent BGA land. If I
tried to place a BGA on the resulting footprint, there is a high
probability of the ball collapse during reflow resulting in a
short.

I just scrapped a prototype run of 60 boards because I forgot to
go back and double check that all vias under the BGA were tented.

With larger pitch BGAs it may be that you can maintain soldermask
design rules even with untented vias. If so, I don't think there's
any absolute necessity to tent the via.

If you're using liquid photoimagable soldermask then the tenting
won't be perfect - the soldermask covers the surface but usually
leaves the via hole open. If you want to ensure complete tenting,
you'll need to specify dry film soldermask. The downside with
this is that it is much thicker than LPI, which may have flow-on
effects in assembly and reliability. e.g. If you need to use
a thin paste screen (because of fine pitch parts), the standard
solder volume deposited for parts like 0402s may be insufficient
because the component will be elevated from the copper by the
thickness of the soldermask. This sort of thing is an issue you
should discuss with your assembler. Long live DFM :-)

As mentioned by others, Protel allows you to tent vias simply
by checking the "tented" check box on the via properties pane.

Cheers,

John Haddy

> -Original Message-
> From: Bagotronix Tech Support [mailto:[EMAIL PROTECTED]]
> Sent: Thursday, 23 August 2001 4:36 AM
> To: Protel EDA Forum
> Subject: [PEDA] tenting vias
> 
> 
> Hello, all:
> 
> I am designing a board with a 388 BGA chip.  I have questions about vias:
> 
> 1)  Should I tent the vias under the BGA?
> 2)  If (1) is yes, should I tent other vias on the board?
> 3)  If (1) is yes, what substance/method is used to tent vias?
> 4)  If (1) is yes, what do I tell the PCB fab house to get them 
> to tent the
> vias?  Is it as simple as "tent the vias"?
> 5)  If blind vias are used, do they need tenting also?
> 
> The BGA has a 1.27mm ball grid.  I am considering a 25 mil pad, 
> 12 mil via,
> 31 mil solder mask opening diameter.  Does this sound good?  If not, what
> would you recommend?
> 
> Best regards,
> Ivan Baggett
> Bagotronix Inc.
> website:  www.bagotronix.com
> 
> 
> 

* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
* To post a message: mailto:[EMAIL PROTECTED]
*
* To leave this list visit:
* http://www.techservinc.com/protelusers/leave.html
*  - or email -
* mailto:[EMAIL PROTECTED]?body=leave%20proteledaforum
*
* Contact the list manager:
* mailto:[EMAIL PROTECTED]
*
* Browse or Search previous postings:
* http://www.mail-archive.com/proteledaforum@techservinc.com
* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *

Re: [PEDA] tenting vias

[rlamoreaux]

4)  If (1) is yes, what do I tell the PCB fab house to get them to tent the
vias?  Is it as simple as "tent the vias"?


You select the vias, and check the box marked tenting in their property
page. The Protel won't remove solder mask in the gerber.

Rob







* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
* To post a message: mailto:[EMAIL PROTECTED]
*
* To leave this list visit:
* http://www.techservinc.com/protelusers/leave.html
*  - or email -
* mailto:[EMAIL PROTECTED]?body=leave%20proteledaforum
*
* Contact the list manager:
* mailto:[EMAIL PROTECTED]
*
* Browse or Search previous postings:
* http://www.mail-archive.com/proteledaforum@techservinc.com
* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *

[PEDA] tenting vias

[Bagotronix Tech Support]

Hello, all:

I am designing a board with a 388 BGA chip.  I have questions about vias:

1)  Should I tent the vias under the BGA?
2)  If (1) is yes, should I tent other vias on the board?
3)  If (1) is yes, what substance/method is used to tent vias?
4)  If (1) is yes, what do I tell the PCB fab house to get them to tent the
vias?  Is it as simple as "tent the vias"?
5)  If blind vias are used, do they need tenting also?

The BGA has a 1.27mm ball grid.  I am considering a 25 mil pad, 12 mil via,
31 mil solder mask opening diameter.  Does this sound good?  If not, what
would you recommend?

Best regards,
Ivan Baggett
Bagotronix Inc.
website:  www.bagotronix.com



* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
* To post a message: mailto:[EMAIL PROTECTED]
*
* To leave this list visit:
* http://www.techservinc.com/protelusers/leave.html
*  - or email -
* mailto:[EMAIL PROTECTED]?body=leave%20proteledaforum
*
* Contact the list manager:
* mailto:[EMAIL PROTECTED]
*
* Browse or Search previous postings:
* http://www.mail-archive.com/proteledaforum@techservinc.com
* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *

Re: [PEDA] tenting vias

[Brian Guralnick]

Yes,

In PCB, go to Tools / Preferences - Defaults - Via.  Turn on tenting. OK, Turn on 
Permanent.  Also, it is useful to save your settings here as well.

This has worked successfully for me.

_
Brian Guralnick



- Original Message - 
From: "Richard Bruer" <[EMAIL PROTECTED]>
To: "Protel EDA Forum" <[EMAIL PROTECTED]>
Sent: Thursday, July 12, 2001 2:01 PM
Subject: [PEDA] tenting vias


| Does anyone out there know if Protel 99SE SP6 can really be set up so that
| the via tenting checkbox is automatically checked when you change layers
| using * ?
| According to the curt email response from Protel tech support (see question
| and answer below), there isn't a way, but I've had mixed results with
| getting good support from Protel, so I figured I'd throw out the question
| here...
| 
| Richard Bruer, P.E.
| Chief Engineer
| Instrument Division
| American Magnetics, Inc.
| 112 Flint Road
| Oak Ridge, TN  37830
| Phone:  (865) 482-1056
| Fax:  (865) 482-5472
| mailto:[EMAIL PROTECTED]
| http://www.americanmagnetics.com
| 
| -Original Message-
| From: Christine Wilinsky [mailto:[EMAIL PROTECTED]]
| Sent: Tuesday, July 10, 2001 4:59 PM
| To: [EMAIL PROTECTED]
| Subject: RE: Tenting vias does not work when using * to switch layers
| 
| Hi,
| Thanks for your inquiry.
| Unfortunately, at this time there is no way to enable a via to always use
| the tenting feature.
| If you have any further questions then please direct them to
| [EMAIL PROTECTED] <mailto:[EMAIL PROTECTED]>
| ---
| Best Regards,
| Protel Support Team
| 
| 
| - Original Message -
| From: "Eric Myers" <[EMAIL PROTECTED]
| <mailto:[EMAIL PROTECTED]>>
| To: <[EMAIL PROTECTED] <mailto:[EMAIL PROTECTED]>>
| Sent: Monday, July 09, 2001 1:57 PM
| Subject: Protel CSC-Web Rpt : Protel Technology Inc (Filename: No File
| Attached)
| 
| 
| > InfoRequest (inserted by WWW page)
| >
| > The following customer filled in the Report Form on the Protel Web site:
| >
| > Customer Name : Eric Myers
| > Customer Email : [EMAIL PROTECTED]
| <mailto:[EMAIL PROTECTED]>
| > Report Type : Question
| > Product Name : PCB Layout
| > Product Version : 99 SE with Service Pack 6
| > Summary : Tenting vias does not work when using * to switch
| > layers.
| > Request Details :
| >
| > License Number is 990009214, Operating System is Windows 98
| >
| > I have my vias set up under Tools>>Preferences>>Defaults for Tenting. It
| > works fine as long as I use Place>>Via. But if I use the '*' while
| > rounting, the via has the tenting turned off. Is there a way to have via
| > always use tenting?
| >
| > Thanks,
| >
| > Eric.
| 
| 

* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
* To post a message: mailto:[EMAIL PROTECTED]
*
* To leave this list visit:
* http://www.techservinc.com/protelusers/leave.html
*  - or email -
* mailto:[EMAIL PROTECTED]?body=leave%20proteledaforum
*
* Contact the list manager:
* mailto:[EMAIL PROTECTED]
*
* Browse or Search previous postings:
* http://www.mail-archive.com/proteledaforum@techservinc.com
* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *

[PEDA] tenting vias

[Richard Bruer]

Does anyone out there know if Protel 99SE SP6 can really be set up so that
the via tenting checkbox is automatically checked when you change layers
using * ?
According to the curt email response from Protel tech support (see question
and answer below), there isn't a way, but I've had mixed results with
getting good support from Protel, so I figured I'd throw out the question
here...

Richard Bruer, P.E.
Chief Engineer
Instrument Division
American Magnetics, Inc.
112 Flint Road
Oak Ridge, TN  37830
Phone:  (865) 482-1056
Fax:  (865) 482-5472
mailto:[EMAIL PROTECTED]
http://www.americanmagnetics.com

-Original Message-
From: Christine Wilinsky [mailto:[EMAIL PROTECTED]]
Sent: Tuesday, July 10, 2001 4:59 PM
To: [EMAIL PROTECTED]
Subject: RE: Tenting vias does not work when using * to switch layers

Hi,
Thanks for your inquiry.
Unfortunately, at this time there is no way to enable a via to always use
the tenting feature.
If you have any further questions then please direct them to
[EMAIL PROTECTED] 
---
Best Regards,
Protel Support Team


- Original Message -
From: "Eric Myers" <[EMAIL PROTECTED]
>
To: <[EMAIL PROTECTED] >
Sent: Monday, July 09, 2001 1:57 PM
Subject: Protel CSC-Web Rpt : Protel Technology Inc (Filename: No File
Attached)


> InfoRequest (inserted by WWW page)
>
> The following customer filled in the Report Form on the Protel Web site:
>
> Customer Name : Eric Myers
> Customer Email : [EMAIL PROTECTED]

> Report Type : Question
> Product Name : PCB Layout
> Product Version : 99 SE with Service Pack 6
> Summary : Tenting vias does not work when using * to switch
> layers.
> Request Details :
>
> License Number is 990009214, Operating System is Windows 98
>
> I have my vias set up under Tools>>Preferences>>Defaults for Tenting. It
> works fine as long as I use Place>>Via. But if I use the '*' while
> rounting, the via has the tenting turned off. Is there a way to have via
> always use tenting?
>
> Thanks,
>
> Eric.

* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
* To post a message: mailto:[EMAIL PROTECTED]
*
* To leave this list visit:
* http://www.techservinc.com/protelusers/leave.html
*  - or email -
* mailto:[EMAIL PROTECTED]?body=leave%20proteledaforum
*
* Contact the list manager:
* mailto:[EMAIL PROTECTED]
*
* Browse or Search previous postings:
* http://www.mail-archive.com/proteledaforum@techservinc.com
* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *