Standardized footprint references

I

Ivan

Guest
Is there a document referencing standards like 1206, 0805, etc. for
component land dimensions?

Also, how can I find these footprints (ie 1206) in Protel?

Thanks one and all for everyone's help.


Ivan
 
Ivan wrote:
Is there a document referencing standards like 1206, 0805, etc. for
component land dimensions?

Also, how can I find these footprints (ie 1206) in Protel?

Thanks one and all for everyone's help.

Ivan
Click to expand...
I have seen pad dimensions in various PCB CAD programs for a number of
SMT parts, and the dimensions were said to come from some standard
(which i will not mention).
I have even seen some nicely done drawings used to justify some of the
dimensions of those pads.
Suffice to say, that pad dimensions go all over the map, from being
smaller (one or both dimensions), thru exactly the size, to excessively
larger than the part lead that would be soldered onto that pad -
especially when one looks at different parts that have the same exact
lead size.
So, as far as i am concerned, the "standard" is not too useful or
functional.
In short, make the lead pads any size you want.

If it were me, i would make *recommendations* and/or *guidelines*,
since nobody seems to give a damn as to what the term "standard" is
supposed to mean.
Start with the pad exactly the size of the lead that would go onto it.
Optionally, add to those X and Y dimensions, any or all of the
following:
1) Add a mil or two for positioning errors.
2) On the edge where a lead bends down toward the solder pad, add one to
three mils for solder meniscus.
3) Add one half of a mil, to one mil for solder meniscus from a given
lead edge to solder pad.
The above three recommendations or guidelines then would give a
minimal pad size that would be workable in almost any shop.
 
"Ivan" <ivanzr1@aol.com> wrote in message
news:4efd11h4jtpcnjshos6ccavemkupfsvshd@4ax.com...
Is there a document referencing standards like 1206, 0805, etc. for
component land dimensions?

Also, how can I find these footprints (ie 1206) in Protel?
Click to expand...

http://ipc.org/

Leon
--
Leon Heller, G1HSM
http://www.geocities.com/leon_heller
 
Thank you for your suggestion and taking the time to reply :)

Ivan




On Sat, 19 Feb 2005 08:35:30 GMT, Robert Baer
<robertbaer@earthlink.net> wrote:

Ivan wrote:

Is there a document referencing standards like 1206, 0805, etc. for
component land dimensions?

Also, how can I find these footprints (ie 1206) in Protel?

Thanks one and all for everyone's help.

Ivan

I have seen pad dimensions in various PCB CAD programs for a number of
SMT parts, and the dimensions were said to come from some standard
(which i will not mention).
I have even seen some nicely done drawings used to justify some of the
dimensions of those pads.
Suffice to say, that pad dimensions go all over the map, from being
smaller (one or both dimensions), thru exactly the size, to excessively
larger than the part lead that would be soldered onto that pad -
especially when one looks at different parts that have the same exact
lead size.
So, as far as i am concerned, the "standard" is not too useful or
functional.
In short, make the lead pads any size you want.

If it were me, i would make *recommendations* and/or *guidelines*,
since nobody seems to give a damn as to what the term "standard" is
supposed to mean.
Start with the pad exactly the size of the lead that would go onto it.
Optionally, add to those X and Y dimensions, any or all of the
following:
1) Add a mil or two for positioning errors.
2) On the edge where a lead bends down toward the solder pad, add one to
three mils for solder meniscus.
3) Add one half of a mil, to one mil for solder meniscus from a given
lead edge to solder pad.
The above three recommendations or guidelines then would give a
minimal pad size that would be workable in almost any shop.
Click to expand...
 
Ivan,
Take a lot of the information you gain here with a grain of
salt. I don't know where Robert gained his experience but by his
comment on allowing for meniscus he must have been dealing with
3-6mil high parts/leads. 1 - 3 mils heel length is totally
inadequate for a normal real world part. He was kinda right about
the IPC land pattern standard, one cannot design land patterns
allowing for the wide variation of manufacturers dimensional
allowances as IPC suggests (i.e. an SOIC lead foot length of
14mil - 50mil, use 32mil as the real length +/- 18mil but forget
the tolerance when designing the land pattern. Do you ever see a
SOIC foot vary by more than 3 times the minimum length in the
real world?). Their system does work pretty good if you design
for the median part dimensions and drop the min and max cases.
SMT Plus' system says the same thing, forget designing for the
max and mins.

I have to think that Robert was talking about a SOIC type
lead but he doesn't state so. Besides SOIC leads there are a
large and varied number of pad requirements for various devices.
Some of those requirements are for soldering, some are for test
and some are for reworkability, good pad designs are a blending
of all three. By the way, for a standard common SOIC lead I would
use 20mils on the toe and heel of the lead, the heal for solder
joint strength (meniscus) and the toe for somewhere to get your
heat into the pad for rework (also works well for a test probe
point). (i.e. a 12mil wide SOIC lead with 22mils of foot, a pad
14 - 16mils wide and 62 mils in length, centered on the
centerpoint of the lead's foot. On small pitch SO devices (also
QFPs, LCCs, TSSOPs and all other small pitch devices) the pad
width will approach the same width as the lead, i.e. 8mil lead
width, pad - 8-9mil width. Sometimes the gap between pads can
take priority over the pad width and drive the pad width right
down to matching the lead width.)

There are too many issues to discuss in this forum but I
would suggest that you look at SMT Plus' literature. I know that
he had two books that he used to sell that discuss land patterns
for SMT devices and runs through a lot of the rules to designing
good SMT land patterns. I have used SMT Plus' system for about 12
years now, it has never let me down through many companies and
across numerous assembly shops.

As for your question about Protel patterns and where to find
them, I don't know because I never use canned libraries. On that
note be warned that Protel libraries do have errors in them. Some
errors are significant, not just borderline issues. Protel does
have some sort of a library listing on their website if I
remember correctly and it is still there. It might be an
interactive utility or spreadsheet.
--
Sincerely,
Brad Velander

"Ivan" <ivanzr1@aol.com> wrote in message
news:t10e11h4n0e4e0m0bup0226qvouqjuegpq@4ax.com...
Thank you for your suggestion and taking the time to reply :)

Ivan
Click to expand...
 
Brad,

Thank you for taking the time to present such a detailed and
informative reply. I greatly appreciate your effort and advice.


Ivan


On Sat, 19 Feb 2005 10:14:38 GMT, "Brad Velander"
<SpamThis@nowhere.com> wrote:

Ivan,
Take a lot of the information you gain here with a grain of
salt. I don't know where Robert gained his experience but by his
comment on allowing for meniscus he must have been dealing with
3-6mil high parts/leads. 1 - 3 mils heel length is totally
inadequate for a normal real world part. He was kinda right about
the IPC land pattern standard, one cannot design land patterns
allowing for the wide variation of manufacturers dimensional
allowances as IPC suggests (i.e. an SOIC lead foot length of
14mil - 50mil, use 32mil as the real length +/- 18mil but forget
the tolerance when designing the land pattern. Do you ever see a
SOIC foot vary by more than 3 times the minimum length in the
real world?). Their system does work pretty good if you design
for the median part dimensions and drop the min and max cases.
SMT Plus' system says the same thing, forget designing for the
max and mins.

I have to think that Robert was talking about a SOIC type
lead but he doesn't state so. Besides SOIC leads there are a
large and varied number of pad requirements for various devices.
Some of those requirements are for soldering, some are for test
and some are for reworkability, good pad designs are a blending
of all three. By the way, for a standard common SOIC lead I would
use 20mils on the toe and heel of the lead, the heal for solder
joint strength (meniscus) and the toe for somewhere to get your
heat into the pad for rework (also works well for a test probe
point). (i.e. a 12mil wide SOIC lead with 22mils of foot, a pad
14 - 16mils wide and 62 mils in length, centered on the
centerpoint of the lead's foot. On small pitch SO devices (also
QFPs, LCCs, TSSOPs and all other small pitch devices) the pad
width will approach the same width as the lead, i.e. 8mil lead
width, pad - 8-9mil width. Sometimes the gap between pads can
take priority over the pad width and drive the pad width right
down to matching the lead width.)

There are too many issues to discuss in this forum but I
would suggest that you look at SMT Plus' literature. I know that
he had two books that he used to sell that discuss land patterns
for SMT devices and runs through a lot of the rules to designing
good SMT land patterns. I have used SMT Plus' system for about 12
years now, it has never let me down through many companies and
across numerous assembly shops.

As for your question about Protel patterns and where to find
them, I don't know because I never use canned libraries. On that
note be warned that Protel libraries do have errors in them. Some
errors are significant, not just borderline issues. Protel does
have some sort of a library listing on their website if I
remember correctly and it is still there. It might be an
interactive utility or spreadsheet.
Click to expand...
 
On Fri, 18 Feb 2005 23:22:19 -0500, Ivan <ivanzr1@aol.com> wrote:

Is there a document referencing standards like 1206, 0805, etc. for
component land dimensions?

Also, how can I find these footprints (ie 1206) in Protel?

Thanks one and all for everyone's help.


Ivan
Click to expand...
IPC-SM-782 is a good starting point. They have an on-line calculator
which is unpleasant to use.

Check manufacturers data sheets and application notes.

AVX has done extensive research on chip capacitors and land patterns.
Look for their "Surface Mounting Guide" for MLC chip capacitors. I
like using their reflow dimensions.
http://www.avxcorp.com/prodinfo_productdetail.asp?I=971&ParentID=124
http://www.avxcorp.com/techinfo_doclisting.asp?Category=Surface+Mount+Capacitors
http://www.avxcorp.com/techinfo_doclisting.asp?PageNumber=1&Pageset=1&Category=Ceramic+Capacitors&SubCat1=&SubCat2=&qry=Select+%2A+from+tblTechInfo+Where+tecCategory%3D%27Ceramic+Capacitors%27+ORDER+BY+tecTopic

PCB Standards has a landpattern calculator. It designs to IPC-782
standards. Check out pcbstandards forums > PCBstandards > Free
Resources > Library Part Documentation for some good info.
http://www.pcbstandards.com/

Mark
 
Mark-

Thank you! The urls that you provided answered many questions,
including those for reflow and wave soldering specs.

I appreciate your attention and help.

Thank you once again,

Ivan


On Mon, 21 Feb 2005 20:30:39 -0800, qrk <SpamTrap@reson.com> wrote:

On Fri, 18 Feb 2005 23:22:19 -0500, Ivan <ivanzr1@aol.com> wrote:

Is there a document referencing standards like 1206, 0805, etc. for
component land dimensions?

Also, how can I find these footprints (ie 1206) in Protel?

Thanks one and all for everyone's help.


Ivan

IPC-SM-782 is a good starting point. They have an on-line calculator
which is unpleasant to use.

Check manufacturers data sheets and application notes.

AVX has done extensive research on chip capacitors and land patterns.
Look for their "Surface Mounting Guide" for MLC chip capacitors. I
like using their reflow dimensions.
http://www.avxcorp.com/prodinfo_productdetail.asp?I=971&ParentID=124
http://www.avxcorp.com/techinfo_doclisting.asp?Category=Surface+Mount+Capacitors
http://www.avxcorp.com/techinfo_doclisting.asp?PageNumber=1&Pageset=1&Category=Ceramic+Capacitors&SubCat1=&SubCat2=&qry=Select+%2A+from+tblTechInfo+Where+tecCategory%3D%27Ceramic+Capacitors%27+ORDER+BY+tecTopic

PCB Standards has a landpattern calculator. It designs to IPC-782
standards. Check out pcbstandards forums > PCBstandards > Free
Resources > Library Part Documentation for some good info.
http://www.pcbstandards.com/

Mark
Click to expand...
 
You must log in or register to reply here.

Welcome to EDABoard.com

Sponsor

Back
Top