Future: 0603 versus 0402 parts

[Haude Daniel]

What helps is to fire up two irons. I touch one side of a resistor with
each, then flick it into a bucket.

Same here. Still difficult with multi-pin parts. But TPH can also be a
botch to rework because you need to liquify (and get rid of) all the
solder that is ob both sides of the PCB and inside the hole.
Single-side is the easiest to rework, but I haven't done that since
my hobby days anyway.

--Daniel

 

[Ian]

I agree, X7R (at worst) every time in my designs where relatively high
capacitance is required.

I suppose if you're building crap consumer products that don't really
have to work much outside of room temperature and you can shave a
teeny bit of cost off it, the 'semiconductor' dielectrics might start
to look attractive-- kind of like the beer goggle effect.

http://news.bbc.co.uk/2/hi/uk_news/scotland/2201198.stm


Best regards,
Spehro Pefhany

As Jim would say "Sn_o_ooort!"

They used _students_ in _Glasgow_?!!
Where'd they find the sober ones?

Regards
Ian

(My daughter graduated from one of the Glasgow Universities
a couple of years ago. The social life is legendary ;-)

 

[Joerg]

Sounds like you must work more in a lab environment than a product
environment. Since all parts need to be approved by purchasing and have
purchasable part numbers as well as alt parts we don't use generic
parts. So a CAD library is 0603_X7R_10V_.01uF not 0603_cap. Also each
ties to a PCB library. So the schematic library is mated to an IPC7351
and 782 (if I got those numbers correct) footprint. If I want to change
footprints I need to change the schematic and ECO back. If I didn't do
it this way I would make an even bigger mess for purchasing. So I need
to make a cad library for each part I use and that library ties be to a
specific part and package size. Also I could care less about lab stock
issues. It is stocking production parts, and pick and place feeders that
is the issue. Takes time and money to swap that roll of 0603 10k parts
out to 0805 10k on the pick an place machine to build a different board.

Well, Cadsoft Eagle is quite smart in that domain: You click on, say, a
resistor, transistor, whatever. Something that comes in various
packages. Provided you created the library correctly that'll give you a
drop-down menu just like Windows Explorer does, with that little plus
sign. Click that and you'll get the package versions. If you discover
after placement that you could get away with a larger version you can
use a routine "change" -> "package". Then it replaces the original part
with a smaller part that has a different ID. This change will also be
reflected when you run the BOM.

Unfortunately Eagle does not yet allow additional part fields. This will
come with the next release, after some petitioning by us industry guys.
So currently it is difficult to do the linking to the partmaster
database. But it is possible via special BOM routines. In Eagle you can
write your own user language program to create, say, a "Hawker-BOM". In
it you can specify how it will merge with part numbers from the
partmaster. The next release should make things easier, then all you
need is the actual partmaster number in a third part field. Since I work
for several clients at a time it would have to be a cross reference
number in my case, or I just create one dedicated set of libraries for
each client.

 

[Hawker]

what you are alluding to here is actually the behaviour of the
dielectric. so-called "high-K" dielectrics are appalling shite - eg Z5U
(worst) and Y5V (not much better). either of these need to run at about
10% of rated voltage to get close to rated capacitance. at 40% rated
voltage its about 40% rated C.....

and for a given capacitance, reducing volume requires higher Er....

and the C-vs-T curve is just as bad (actually a bit worse), in either
direction. So even if you massively over-rate the component voltage,
unless your design sits at 25C all the time, you will still take a beating.

Several times I have done an exercise where I compare Z5U/Y5V with X7R,
and for a real product with real temperature swings, X7R wins every time
(most capacitance in a given package). I really dont know why anyone
ever uses Z5U/Y5V.

Cheers
Terry

Actually I am not. I am fully aware of what you speak of, but the report
I read compared X5Rs to X5R and X5R is pretty close to X7R except at
temp exreams.

Hawker

 

[Hawker]

For lab stock I can understand this but for the CAD library? My CAD
allows to generate a part and then designate as many package styles as
you want. So, for example, I can place 100K pull-up resistors in 0603
and when it ends up looking like L.A. at rush hour I can tell the CAD
software "Let's make all these 0402".

Sounds like you must work more in a lab environment than a product
environment. Since all parts need to be approved by purchasing and have
purchasable part numbers as well as alt parts we don't use generic
parts. So a CAD library is 0603_X7R_10V_.01uF not 0603_cap. Also each
ties to a PCB library. So the schematic library is mated to an IPC7351
and 782 (if I got those numbers correct) footprint. If I want to change
footprints I need to change the schematic and ECO back. If I didn't do
it this way I would make an even bigger mess for purchasing. So I need
to make a cad library for each part I use and that library ties be to a
specific part and package size. Also I could care less about lab stock
issues. It is stocking production parts, and pick and place feeders that
is the issue. Takes time and money to swap that roll of 0603 10k parts
out to 0805 10k on the pick an place machine to build a different board.

Hawker

 

[RST Engineering \(jw\)]

Joerg ...

It is too bad that Protel killed off Circuitmaker/Traxmaker. The folks up
here in Grass Valley that wrote Parts & Vendors had a "give me your
circuitmaker.bom file and I'll translate it to your part number in P&V".
Now P&V has a dozen or so "User Fields" for each part number, into which you
could store, for example, Client1PN, Client2PN, and so on. WItht his you
could give your customer their own ready for prime time parts list.

Just a thought, mindya...

Jim

Unfortunately Eagle does not yet allow additional part fields.

Since I work

 

[Joerg]

Joerg ...

It is too bad that Protel killed off Circuitmaker/Traxmaker. The folks up
here in Grass Valley that wrote Parts & Vendors had a "give me your
circuitmaker.bom file and I'll translate it to your part number in P&V".
Now P&V has a dozen or so "User Fields" for each part number, into which you
could store, for example, Client1PN, Client2PN, and so on. WItht his you
could give your customer their own ready for prime time parts list.

Just a thought, mindya...

I haven't done this with Eagle yet but supposedly you can do it. BOM
routine spits out linkable BOM, this links with Access type data base,
from there you'd run the Client1PN report or Client2PN report.

 

[John Larkin]

I haven't done this with Eagle yet but supposedly you can do it. BOM
routine spits out linkable BOM, this links with Access type data base,
from there you'd run the Client1PN report or Client2PN report.

PADS has lots of slots for part attributes. We use generic resistors
like RES/0805 and then fill in the VALUE and HTI# (highland part
number) fields on each part. PADS will then run a script file to make
a bom in our format, and also can be persuaded to make a solder
stencil and a pick-n-place coordinate file.

John

 

[Joerg]

PADS has lots of slots for part attributes. We use generic resistors
like RES/0805 and then fill in the VALUE and HTI# (highland part
number) fields on each part. PADS will then run a script file to make
a bom in our format, and also can be persuaded to make a solder
stencil and a pick-n-place coordinate file.

They were ahead of the pack, as was OrCad which had eight attribute
fields even way back in the DOS days. Eagle doesn't yet and it took some
convincing but we were promised it'll come. Most of us need at least one
more than the usual two because there can be parts that have identical
packages and names but, for example, one is screened for avalanche
voltage range or manufacturer or something like that. Right now I must
give it another name.

For me there is only one gripe left WRT Eagle but that is a major one.
It does not allow hierarchical sheet structure. Not a good thing but
Cadsoft doesn't seem to think it's important. Anyone who has done med or
gvt work knows that it is.

 

[MassiveProng]

I like flat.

Did you mistakenly set your PC two hours ahead?

 

[Joerg]

Hierarchical schematics make some sense for things like FPGAs. But
every part on a board has a reference designator and a physical
existance, so how do you handle hierarchy? You can't have 10 R1's, can
you? Some other naming convention?

In a typical hierarchy in the med industry the top sheet does not
contain any parts. Maybe a house-keeping chip, RFID or a regulator but
usually not. It contains 5-10 blocks that split the board into
functional units. Each block has all the ports it needs and there are
actually buses and nets going from one to the other. All of them. Now
you can double-click on, say, the phase shifter block and it opens up
the page with the circuitry. It has the same port pins. OrCad actually
pinged me whenever I forgot one. Oh, do I miss that.

I like flat.

I like hierarchical

 

[John Larkin]

They were ahead of the pack, as was OrCad which had eight attribute
fields even way back in the DOS days. Eagle doesn't yet and it took some
convincing but we were promised it'll come. Most of us need at least one
more than the usual two because there can be parts that have identical
packages and names but, for example, one is screened for avalanche
voltage range or manufacturer or something like that. Right now I must
give it another name.

For me there is only one gripe left WRT Eagle but that is a major one.
It does not allow hierarchical sheet structure. Not a good thing but
Cadsoft doesn't seem to think it's important. Anyone who has done med or
gvt work knows that it is.

Hierarchical schematics make some sense for things like FPGAs. But
every part on a board has a reference designator and a physical
existance, so how do you handle hierarchy? You can't have 10 R1's, can
you? Some other naming convention?

I like flat.

John

 

[John Larkin]

Did you mistakenly set your PC two hours ahead?

It shows the correct time, but it is running XP, so any stupidity is
possible. It's a crap Dell, soon to be replaced by an HP raid-ed
server box, so I don't much care.

John

 

[MassiveProng]

It shows the correct time, but it is running XP, so any stupidity is
possible. It's a crap Dell, soon to be replaced by an HP raid-ed
server box, so I don't much care.

Next time you boot, see what the actual BIOS has it set to.
Sometimes that and the OS differ from each other.

 

[Glen Walpert]

On Thu, 15 Mar 2007 17:46:21 -0800, John Larkin

Hierarchical schematics make some sense for things like FPGAs. But
every part on a board has a reference designator and a physical
existance, so how do you handle hierarchy? You can't have 10 R1's, can
you? Some other naming convention?

I like flat.

I hate flat, except for the smallest of designs, and would never
consider using a CAD system which does not support hierarchy. (I am
currently using Protel). I typically use 3 digit part numbers, where
the first digit identifies what block (sheet) the part is in, and the
last two which part in the block. If there are more than 10 blocks I
will use 4 digit part numbers for blocks 10 and up. Since the parts
are grouped by function both on schematics and board layout, this
numbering system makes finding parts on the board easy, and a design
that really benefits from hierarchy will usually have enough parts
that 3 digit part numbers are required anyhow (at least for passives).
Where all or most of the blocks have less than 10 ICs I will use 2
digit IC numbers done the same way. If you screw up and use the same
part number twice, DRC will let you know.

This lets you put a design with thousands of parts on paper small
enough to print on a cheap laser printer, and small enpugh to easily
handle when debugging.

 

[Robert Latest]

Each block has all the ports it needs and there are
actually buses and nets going from one to the other.

Speaking of ports: Eagle doesn't really have any. Very annoying, not just
with the (non-extant) hierarchical sheets but also with simple multi-page
ones. Of course you can give net segments on different sheets the same name,
and you can also label them, but if you mess around with your schemtic too
much you may lose tracks of nets and labels.

I've once written a ULP that automatically labeled all net end lines that
ended without being connected to anything, but it doesn't work right
(because you never know which way up the label comes out).

I'm looking forward to the additional data field feature. Hopefully it's at
the schematic level as well as on the library level, although in the latter
case you can kludge around the limitations by putting the requited data into
the "description" field and extract it via a ULP.

robert

 

[Joerg]

Joerg wrote:




Speaking of ports: Eagle doesn't really have any. Very annoying, not just
with the (non-extant) hierarchical sheets but also with simple multi-page
ones. Of course you can give net segments on different sheets the same name,
and you can also label them, but if you mess around with your schemtic too
much you may lose tracks of nets and labels.

I would have stayed with OrCad. However, when at companies it crashed on
me too often and the price went up more than 3x since SDT just for
schematic entry. Eagle hasn't crashed once.

I've once written a ULP that automatically labeled all net end lines that
ended without being connected to anything, but it doesn't work right
(because you never know which way up the label comes out).

I'm looking forward to the additional data field feature. Hopefully it's at
the schematic level as well as on the library level, although in the latter
case you can kludge around the limitations by putting the requited data into
the "description" field and extract it via a ULP.

IMHO it wasn't a good decision not to offer hierarchical on the next
release but who am I to say.

 

[Rich Grise]

On Thu, 15 Mar 2007 17:46:21 -0800, John Larkin


I hate flat, except for the smallest of designs, and would never
consider using a CAD system which does not support hierarchy. (I am
currently using Protel). I typically use 3 digit part numbers, where
the first digit identifies what block (sheet) the part is in, and the
last two which part in the block. If there are more than 10 blocks I
will use 4 digit part numbers for blocks 10 and up. Since the parts
are grouped by function both on schematics and board layout, this
numbering system makes finding parts on the board easy, and a design
that really benefits from hierarchy will usually have enough parts
that 3 digit part numbers are required anyhow (at least for passives).
Where all or most of the blocks have less than 10 ICs I will use 2
digit IC numbers done the same way. If you screw up and use the same
part number twice, DRC will let you know.

This lets you put a design with thousands of parts on paper small
enough to print on a cheap laser printer, and small enpugh to easily
handle when debugging.

I've even seen functional modules outlined in(on?) the silkscreen, and
identified ("RF amp", "mixer", "IF amp", "Detector", etc.)

Cheers!
Rich

 

[John Larkin]

On Thu, 15 Mar 2007 17:46:21 -0800, John Larkin



I hate flat, except for the smallest of designs, and would never
consider using a CAD system which does not support hierarchy. (I am
currently using Protel). I typically use 3 digit part numbers, where
the first digit identifies what block (sheet) the part is in, and the
last two which part in the block. If there are more than 10 blocks I
will use 4 digit part numbers for blocks 10 and up. Since the parts
are grouped by function both on schematics and board layout, this
numbering system makes finding parts on the board easy, and a design
that really benefits from hierarchy will usually have enough parts
that 3 digit part numbers are required anyhow (at least for passives).
Where all or most of the blocks have less than 10 ICs I will use 2
digit IC numbers done the same way. If you screw up and use the same
part number twice, DRC will let you know.

This lets you put a design with thousands of parts on paper small
enough to print on a cheap laser printer, and small enpugh to easily
handle when debugging.

We do everything B-size, 11x14", which is easy to handle and read, and
punches/folds into a loose-leaf binder nicely. The biggest board I've
done is something like 25 sheets, 1200 parts maybe, with sheet 1 being
the block diagram and table of contents. I wouldn't like to silkscreen
things like "R1531" next to every 0603!

We always resequence the ref desigs in physical order, to keep
manufacturing happy.

John

 

[John Larkin]

I've even seen functional modules outlined in(on?) the silkscreen, and
identified ("RF amp", "mixer", "IF amp", "Detector", etc.)

Cheers!
Rich

We do that. And draw boxes around channels, and number them, and put
text directions near switches and stuff, if there's room.

And we always say *what the board is*. I hate to find an interesting
flea-market board that doesn't say what it is.

John