PCB designing for 6 layer

Layout
43

true

but i would assume the centerline as below

957Ɨ333 31.1 KB

44

969Ɨ450 61 KB

45

I would put the center(line) where the center has been specified by the manufacturer (not the case here afaik) OR where the FPC cable ends in the device.

The FPC cable ends 2.1 mm from the ā€˜insertion edgeā€™ inside the device.
From the insertion edge itā€™s 4.9 mm to the lever side of the device and as per the side drawing the pins stick out a further 0.3 mm (0.6 - (5.2 - 4.9)).
The y dimension of the pads is 1.1, where as the pins are 0.6 mm, normally centered this would give a distance of 0.25 mm to in vertical direction to the pad edge, but they specced 0.2 mm at the ā€˜upperā€™ side there. This means the pad center is vertically shifted down by 0.05 mm vs the pin center.
So the (negative) y value for the pads then comes to 2.75 mm (4.9 - 2.1 - 0.05).

46

Thatā€™s OK, not perfect, but OK. Always work from the dimensions, never from what you see, unless you have no other choice.
They just forgot to put in those separation marks, that tell the reader that the drawing only shows the most right and left parts with some pins and leaves out the middle of the device, that is just repetitiveā€¦

1 Like
47

centerline was a bad word by me

i meant just reference line or something to align body to pads in this specific case

1 Like
48

Omron_XF2M_0.5_40P_SIDE.kicad_mod (7.2 KB)

1024Ɨ506 90.8 KB

1 Like
49

but two pads 41 that are not next to each others is not nice

technically they belong to the same net

if kicad was strict would create an open net unless connected

50

thanks Joan

one question

  1. how important is F.Fab outline and designator because most components from Kicad do not have F.Fab layer is it important from PCB manufacturing point of view or from PCB designing point of view.

Regards

51

Hmā€¦ I usually just use a generic 41 pin symbol and use pin 41 to connect to groundā€¦ others might use a more sophisticated symbol that will depict pin 41 as housing ground or etcā€¦
How would you number them?

52

You need to ask that the guys with more experience than meā€¦
I went over my private libs about 2 months ago and added F.Fab - I had that info on Dwgs.User/Cmts.User before and F.CrtYd was added by me as well then and there.
I then checked the boards I already did by swapping the footprints for the upgraded ones and found, that I placed most devices with Courtyards touchingā€¦ if any of those boards would need to go to an assembler this will be very important.
F.Fab is needed for me to see the layout in 2D. I canā€™t do without those device outlines anymoreā€¦ just pads is not enough and the Silkscreen layer is OFF when I do layout as itā€™s distracting and lacking information.

1 Like
53

it was 42 pins

40 signals and 2 dummies

the dummies should probably go nowhere
in some cases atleast they should not go to ground or anywhere

so i would just follow from last siggnal 40 to 41 and 42

ps
in mentor tools when you draw 2 pads with same pin-number in footprrint editor (cell) you acctually get a ratsnet in footprint editor between the 2 pads
ds

54

PCBnew does similar stuff for same numbered pads in a layout when you connect only one of the pins to the respective netā€¦

1 Like
55

makes perfect sense

they are the same net

and if not intended to go to gnd it will give an open net

and you dont want to route a trace just to clear that

56

thanks nicholas even if i number those pads as 41 and 42 they are not connected to any thing does kicad not complain saying these pads are not connected any where

57

@Nick123
In case you want to use that fp, download it again (I updated it up there)ā€¦ the create-a-new-footprint-wizard screwed me over with the reference fieldā€¦ I just edited the file and made it how I think it should be:

  • REF** on F.Fab (built in reference field)
  • %R on Eco1 (text field)
  • %R on F.Silk (text field)

That way one can switch off Silkscreen during layout and also disable reference/value in render tab during layout, without loosing the F.Fab outlines infoā€¦

The wizard had confused meā€¦ REF** was on F.Silk and %R on F.Fab (I also had %R the wrong way around and put in R%).
:flushed:

58

no because they are not connected in the schematics

2 loose pins without connections in the netlist

59

thanks nicholas i got it

60

Joan Sparky

in this diagram F.Fab(yellow line) crossing over on both pads 41 does this not impact the signal on that pad
lets assume for now if 41 pad was a real signal pad connected to some X pin to the processor ?

Regards
nick

61

so basically F.Fab is for our easy while doing the PCB designing just wanted to make myself clear that this layer is not needed by the PCB fabricator

62

The only layers that are needed to make a pcb are:
x.Cu (and other copper layers if more than 2 layers)
x.Mask
If you want silkscreen, then you also need
x.Silk
If you want a solder paste stencil you also need
x.Paste
If you want to define the outline of the board (otherwise boardhouse just uses rectangular largest dimensions that keep all the stuff above ā€˜on boardā€™) you will also need
Edge.Cuts
Youā€™ll also be able to output a drill file if you put down vias or through holesā€¦

Any other layer is for documentation or assembly or layout help and will not do anything to the gerber output afaik.
x.CrtdYd is for you to make sure you donā€™t put one device into another and/or give the assembly machine enough space to put the SMDā€™s down
x.Fab is for you during layout or someone else as documentation later which device sits where and how