Orcad Layout and BGAs

[bob treacy]

Hi,

I had been using the OrCad Layout Knowledge Exchange, but they decided to quit hosting it. With luck, maybe some of that group has shown up here, or will in time.

I am working with an engineer on a BGA layout and we have not selected a package yet. We are looking at a choice between 1.00 mm and 1.27 mm pitch parts. I would like to know what the tradeoffs are between the two parts in general. However, I would also like to know if anyone has done any of the 1.00 mm parts in Layout and if so, is it worth it to use a via in the pads at this pitch or is that only a benefit for finer pitch parts? As far as I know, the only other approach is a 'dogbone' fanout. Is there any other way to handle a layout with these BGAs?

[Tom]

Bob,

I would go with the 1mm pitch device. You can still use a through hole via without any problems.

Here are the specs for a 1mm pitch BGA:

Pad Size - 0.45mm (18 mil)
Via Size - 0.55mm (22 mil)
Via Hole - 0.25mm (10 mil)
Single Track Trace Width - 0.15mm (6 mil)
Double Track Trace Width - 0.10mm (4 mil) Note: the via would have to be 0.50mm

[bob treacy]

Tom,

Thank you for the reply. By the way, this is a very nice website. It looks to have been quite an effort to put all these forums in place. There was a lot of information in the OrCad archives that simply is no longer accessible.

In our current project we have kept everything above 6/6 so far which seems to be a good threshold to avoid premium PCB fees (generally trying to meet IPC level 2/class B) This is the first BGA design and I don't know if it is practical to select the 1.27 mm package and expect to continue with 6/6. However, I guess with enough layers anything is possible.

The OrCad library only has a few BGA footprints on 1 mm pitch. Even though they are metric parts, they are still saved in an english dimension format. The pad size is 24 mils (30 mil pad on the 1.27 mm parts). You suggested 18 mils for a 1 mm part. I would think that a small pad size would make the part indexing more critical, but probably result in less bridging. How did you arrive at an 18 mil pad? Is there perhaps an IPC guideline for this that OrCad may not have tried to match?

I have been doing this stuff for about two years. The smallest PTH size I have used so far (without a premium) has been 20 mils on .062 and .090 boards. Where does your board fabricator start to put a premium on a small hole size? Is 10 mils on .062 and .090 PCBs pretty acceptable to most board shops these days? This stuff changes so fast, it seems what was a premium not long ago can quickly become standard if you don't pay real close attention.

By the way, being able to edit after posting is a nice touch. Sometimes no matter how long you look at something...

-Bob

[Tom]

Bob,

The common industry formula for calculating BGA Pad Size is:

50% of Pin Pitch +/- .05mm (.002")

We do all of our designs, placement & routing in metric, so I would naturally pick the 1mm pitch BGA. I am working with IPC & NIST in the transition process to eliminate the English measurement system from the EDA industry.

Check out http://www.nist.gov/metric

Soon, the only parts that will be available will be metric based parts. JEDEC, IPC, ANSI, EIA, NIST, IEC and all the standard groups have already switched all there documentation to metric. The component assembly lines are all being tooled for metric.

[randychase]

Originally posted by bob treacy
Tom,

Thank you for the reply. By the way, this is a very nice website. It looks to have been quite an effort to put all these forums in place. There was a lot of information in the OrCad archives that simply is no longer accessible.
-snip-
By the way, being able to edit after posting is a nice touch. Sometimes no matter how long you look at something...

-Bob

Thanks Bob, that was one of the reasons we did this site. We eventually intend on creating a body of knowledge for everyone to use.

And yes, being able to edit or delete your post is very nice compared to email.

P.S. If there is enough interest, I would be happy to create an Orcad forum grouping here.

[TonyQ]

I am in a similar situation. We are going to a faster DSP and that means moving from a 240pin TQFP to a 400-ball 1.27mm pitch BGA package. This will be my first BGA design. Due to the low volume nature of our business, I am thinking of using a PGA footprint and using a BGA to PGA conversion socket, at least for the first revisions.
By the way, I use Orcad Capture & Layout on my PCB designs. I work stricktly in metric. I hope that there's enough Layout people out there to start a Layout forum here.
-Tony

[TonyQ]

To be fair to Cadence, it is posted somewhere that the Knowledge Exchange database was taken off-line because it was hit by a virus. It looks like all the database got destroyed.

Tony

[Jackie Oh!]

Hi Tom and everyone,

I have to build a 160 pin .8mm pitch bga in Orcad Layout...a couple of questions.

Should I be using micro vias/via in pad? or can I get away with dog-boning. If I can dog-bone, how small do I have to make routes, pads, vias?

If I have to use micro vias...Bob, how did you set up the padstacks in Layout? Did you have to do any extra gerber tricks with the pads or holes? What about via in pad? Did you do that on your 1mm pitch BGA?

And how many layers will I have to use? This is a RF board which means I have to route power - no plane.

My stack up for a 6 layer board is generally like this:

Top - components and as much ground pour covering as possible
GND
In1
GND
In2
Bottom - all GND - no components.

I would suspect that it'll have to be a similar type of stack up if I have to add layers.

I'd like to get this right the first time. Any and all advice/help is appreciated!

Jackie Oh!

P.S. Tom, I know I've seen posts on .8mm pitch bga's on the site, but can't seem to find them now...I know you're always really busy, but when you get a couple of minutes, would you please link me to them? Thanks again for your help.

[Tom]

Please see the attached file.

[Jackie Oh!]

Thanks alot Tom! It's a big help.

Jackie Oh!

[Tom]

Jackie,

I also have great metric fanout solutions for metric pitch QFP's and TSOP's that I created for the IPC Expo in Long Beach, CA where I gave the Keynote Address at the IPC Designers Summit.

Let me know if you would like me to send them to you.

[qrk]

I made a BASIC program to generate BGA footprints with via dispersion. It's a bit clumsy to use as you alter the source code to change parameters. However, you can generate the basic footprint in a couple minutes. Adding the silkscreen info will take longer. Program generates an ASCII MIN file. Instructions are in the comments. Hope someone finds it useful.