PCB footprint check

Layout
1

Hi,

I am using this http://www.onsemi.com/pub_link/Collateral/AR0330CM-D.PDF. On Pg 70,71 thee is footprint information. I created a footprint using the footprint wizard. Could someone please check this?

I am unable to upload the file here so I have saved it at http://expirebox.com/download/d74c408497ff16f8cbc4bdcc93c26a6b.html

If there is some other place to put my files please let me know

2

Your F.Silk lines are not up to scratch… why didn’t you just change the gridsize to something bigger like 0.1 or 0.2 mm and did one line per side? - it doesn’t need to be 100% on the housing dimensions, as those have errors and the silkscreen has got a placement error that is even worse…

ball-pitch is OK.

ball-pad size… no idea, any datasheet for that? The ones from OnSemi for that exact housing are empty… might want to write to a sales person/distributor to get the recommended footprint for a part like this?
Judging from a ‘similar’ package (pitch 0.5 mm, 64 pads, https://www.onsemi.com/pub/Collateral/567HW.PDF) the pads seem to be ~20% larger than the balls… (0.22 vs 0.27).
Means, if the ball diameter ‘D’ is given as 0.25 on page 71 of the AR0330CM datasheet you’d want to go for 0.3mm pad diameter… you got 0.25 mm - not enough to make soldering more successful.

Here you go (you need to change VAL/REF specifics to what you need, I just did them as I use them and this is not KiCAD conform):
BGA_64_0.65.kicad_mod.zip (848 Bytes)

960×540 120 KB

1 Like
3

Awesome. Thanks for the help. I didnt know the pad ball size has to be larger. Second, what is that green user.cmts layer ? Is it for comments? When you say change VAL/REF designators, you just mean the reference designators correct?

4

It’s for whatever you want :smile:
In that case there I marked out the area where the receiving pixels of that CMOS are… but I forgot to mark the center coordinates with a crosshair. My bad.

This footprint doesn’t obey the rules that KiCAD librarians have set, nor would anyone else approve them.

  • The 1st pin marker is under the IC once soldered - bad for post-production check up, at least it’s not a circle (had one batch pcb come back from china with circles in F.Silk missing some time ago).
  • REF** field should be on F.Silk and bigger, so you can put it besides the IC for placing the components/whatever - good fr checkup, maintenance.
  • The housings outline is usually not on Dwgs.User… but some other layer.
    Stuff like that.
    I have my reasons why I do it this way, but that’s me.
    As I reworked that footprint I added it to my lib, so I obeyed my private standard, but uploaded it for you so you can (with some little tweaking) get it back to KiCAD/whatever standard you like but with the improvements.
5

Thats interesting. I am trying to do the silk screen from my orginal footprint again. But I find it hard to know where to stop. I know the length of each side, but to draw it accurately is hard? How do you draw it so fast? Also, how did you draw the active are correctly? What are the dimensions you take as a reference?

6

drawing accurate:

  1. set the grid to the smallest stepping you need (within reasonable limits)
  2. grab the polygon tool and let go off your mouse
  3. observe the absolute coordinate readout at the bottom of the screen (to the right are the relative ones)
  4. use the arrow keys to move to the first coordinate (observe readout)
  5. hit [ENTER]
  6. use the arrow keys to move to the next coordinate (the finer the grid, the slower)
  7. hit [ENTER]
  8. repeat 6/7 till you got the outline/whatever closed
  9. take the mouse again and move somewhere
  10. click [right mouse button] and select ‘End Polygon’
    …if lines should be on another layer with another thickness…
  11. hover over line, hit [E]
  12. hit [TAB] 4 times and type in new line thickness (dot-zero-five for 0.05 for example)
  13. hit [TAB] 2 more times and hit the first letter for the layer you want this line on ([D] for Dwgs.User for example)
  14. repeat 11-13 until you’re happy

Thicker lines are easier to select with [E]… anything below 0.05 needs zooming.
If you need (as I did there) same lines on different layers, just select them with the mouse (click&hold top left, move and let mouse go at right bottom) and copy the block somewhere to the side (with the selection active and moving with your cursor, hit [right mouse button] and select copy block), then delete elements you don’t want, change lines to different thickness/layer and move the block back as a whole.
You can speed up that operation by choosing a lower res grid - the block selections movement will snap to the grid and land back over the ‘original’ - you won’t need to fiddle.

The coordinates for the housing were given on page 70/71 as A (6.278) and B (6.648).
In absolute coordinates you just divide those by 2 (for centered placement) and round off to match your grid settings… so 6.278/2 = 3.139 ~ 3.14

1 Like
7

Awesome. Thanks for the help

8

If you do non-centered stuff you want to use the relative coordinate readout… observe that those reset to (0,0) for your current cursor position when you hit [SPACE]

9

I will try that out too. Thanks for the help

10

I just switched to Cairo and see that the FPaste layer touch each other. Is this okay?

11

I think that’s the pad clearance (min distance for tracks or other pads around it) as long as they don’t overlap OTHER copper pads/tracks all is fine.

My KiCAD feels bonkers atm for me in this regard. I couldn’t get a real grip on the pad clearance, soldermask clearance and paste clearance. I just set them pretty small so the footprint looked alright in 3D… needs observation when being placed onto a pcb for sure.