PCB designing for 6 layer

The pad on pcb should ideally be same pad size as on the chip.

Waist of the ball is as you point out wider.

Rarely the data sheet reveal the chip pad size, but most times they have a recommended footprint.

thanks keruseykaryu

this is answer to my own question also answered by keruseykaryu

this is for all who will ask why 0.35mm pad size on PCB of 0.45mm ball diameter on chip
the answer is in the bellow link
http://processors.wiki.ti.com/index.php/General_hardware_design/BGA_PCB_design

Regards

Hello guys

In the picture bellow
i have seen few of the kicad_mod files where in the
the F.SilkS line touching the pad and also the F.fAb touching the pad
Questions:

  1. what is the importance of these 2 layers?
  2. And how does this impact the PCB manufacturing ?
  3. do these layers block the data/signal flow?

Read from here:

Fabrication Layer (very important)
… should depict the housing outline (sans pins) for placement in the layout tool and pin #1 marker

Courtyard Layer (important)
… should outline devices maxium extension (housing WITH pins) plus safety space, use as placement/spacing help when you position parts… should never overlap from one device to the other

Silkscreen Layer (not so important)
… anything you want to appear on the finished board in the silkscreen, pin #1 markers, outlines, information, etc.pp.
Keep away from pads.
Might pay off to have pin #1 marker for visual inspection after fabrication, etc…
Important for manual placing of BGA devices.

2 Likes

Agree.

Remember, fab layer must have reference designators. %R

Unfortunately in kicad this is up side down world.
It’s mandatory and default on silk but not fab.
Should be mandatory for fab, optional for silk and default for both.

%R in both cases.
Not REF** for one and %R for the other.
Confusing and no extra value.

Courtyard in Mentor is called place keep out.
No other component can intrude with its own place keep out inside.

There is also a route keep out layer.
Some components forbid routing under certain areas.

Unfortunately not seen this in kicad.

so that means this is wrong

  1. FPC_40(yellow text) represents the F.Fab in the bellow image
  2. border( sky blue surrounding all pads) is the F.SilkS

can someone please explain me what is correct then

fab layer should preferably contain the part outline itself from the datasheet
preferably pretty detailed
also a pin 1 marker if that makes sense for the part
add text %R to fab layer so you get ref des in fab layer also

once you made a drawing of the part on fab layer it becomes more easier/natural to see where to put your silkscreen outline
silkscreen should also include a pin 1 marker, either the disigt “1” sometimes more digits d indicate the numbering
or an arrow made with lines or a circle, same goes for fab layer

an example where i turned of the pads to show the detailed fab layer

ps
the reason “SW-64-2” is so yellow is because it set to invisible
i dont want to see value in layout
ds

2 Likes

so this F.fab(yellow) represents where the component is placed by the PCB manufacture is that correct ?

so in that case is the bellow drawing correct ?

it may very well be

cant say without seeing the datasheet of the part

but looks reasonable

%R should normally translate into whatever text you have in refdes

you can (for reasons unknown) change the REF** text to anything and it will get reflected into your %R text

in summary: your %R should be translated into REF** behind the curtains of kicad

as it read %R i think is a bit strange

example

possibly you changed the predefined value into %R

not good

just add a new text from the toolbar to the right as in my picture

dont alter value mandatory text
just make it invisible if you are like me :slightly_smiling:

clarified a bit more

dont put pad 0 on both unused pads

because technically they will become the same net (even if kicad today maybe not act that way)

and if you dont connect them on pcb they will give an open net.

possibly dosent happen in kicad today, but i would give them different pin numbers or possibly no pi-number at all

1 Like

hey nicholas i think it is completely wrong i mean the 2nd design that i uploaded but the first design was correct

i will tell you the reason this is because

  • it is designed using the standard footprint wizard FPC connector.

  • if i see its 3D footprint i see the bellow image in which i can already see the F.Fab layer and other details
    see bellow you can see yellow lines so i guess the F.Fab layer is already integrated by Kicad which is not visible in the footprint but i am not sure what i am saying is correct or wrong can some one please show some light on it

i feel first design is correct the second design that i upload based on nicholas information i feel that is not needed
now the only thing missing is the pin 1 marking but for PCB manufacturer he need not know Pin 1 marking because he has to just place it as per this design now the pin 1 marking may be needed by the PCB designer that is for me to do the routing but if i can see the pad numbers then i need not know the pin 1 marking now once the PCB is manufactured the pin 1 marking needs to be known to some testers and so on in that case i can add pin 1 marking using a F.SilkS

let me know your feedback guys also nicholas can you show some light on this one

cant say

i dont use either wizard or 3-d models

nor do i know what fpc means

i work from manufacturers datasheet

so please provide manufacturer of the part and part-number

1 Like

The footprint from the wizard is missing:

  • pin 1 marker on F.Fab (and F.Silk if you need it)
  • a projected drawing of the device on F.Fab
  • reference field on F.Fab
  • if the flat flex cable needs free space on the board there should also be some information aout this on either Dwgs.User or Cmts.User for you as a help during layout

Assuming the pink rectangle in the background is F.Crtyd, then that’s there at least.

1 Like

hi nicholas
please find in the link bellow

http://www.mouser.com/ds/2/307/en-xf2m-845115.pdf

the wizard and your result do not resemble the connector outline according to datasheet well at all

if i had my way Omron parts should be under github/kicad/footprints/Omron/part-number
not somewhere under /connectors/fpc/blablabla

sorry for the OT rambling at the end here

i suggest you crank up the footprint editor and add the footprint to your collection
also make a pull towards github (that will go neglected for ages)

sorry, i have an JAE similar but not Omron

i typically extend the courtyard to cater for the flex-cable radius and human fingers to put it in.

some flex-cable connectors get the cable very close to the pcb so not even 0402 can get the height needed.
and unfortunately kicad dont have the capability to add height restriction zones (but i can forgive that easily)

1 Like

The datasheet misses the relative distance/position of the footprint vs the device, or I am to dumb…

[edit]
I will assume that the little rectangles in the pads for the pins are actually the pins and the 0.2 mm distance of the pad edge to the pin edge is the needed information. Very risky if an assembler needs to depend on this - can only hope there is some additional packaging drawing that depicts device vs footprint vs position in tray/reel …

thanks Joan

pin1 marker is not needed but let me add in F.SilkS for testing guys just in case needed
reference filed on F.Fab i probably need to add as per nicholas explanation

projected drawing of the device is already shown in the 3D view now i don’t know whether the PCB manufacturer will be able to see it or not

thanks nicholas can you explain how they do not resemble