• State Resolved
  • Locked Locked
  • Replies 4 replies
  • Answers 1 answer
  • Subscribers 64 subscribers
  • Views 618 views
  • Users 0 members are here
Support feedback
Options
Options
Related

This thread has been locked.

If you have a related question, please click the "Ask a related question" button in the top right corner. The newly created question will be automatically linked to this question.

LMG1205: DSBGA layout and stackup

Mike Twieg
Intellectual 960 points
Part Number: LMG1205

I'm seeing some vague and contradictory info regarding layout of the LMG1205. On one hand, there's AN-1112, which says the following on page 6:

"2. A copper layer thickness of less than 1 oz is recommended to achieve higher solder joint stand-off. A 1 oz. (30 micron) or greater copper thickness causes a lower effective solder joint stand-off, which may compromise solder joint reliability.

3. For the NSMD pad geometry, the trace width at the connection to the land pad should not exceed 2/3 of the pad diameter."

On the other hand, I'm considering the design files for TI's LMG1205 evaluation board, LMG1205HBEVM. That design shows the following:

1. Specifies 2oz copper on all layers, including the component layer.

2. Uses NSMD pads, but uses wide polygons to connect to the pads, some of which are at least as wide as the pads.

Obviously since the LMG1205 is made for high power density DC-DC converters, it's very convenient to use larger copper features than. But are we supposed to entirely ignore AN-1112? What guidelines are we meant to follow for the LMG1205?

Also, do the copper weights mentioned above refer to starting or finished thickness (including the plating)?

Regards,

Mike

  • 0
    TI__Guru**** 189401 points
    Hi Mike,

    To achieve the performance specified in the LMG1205 data sheet, please copy the EVM as close as possible.

    As you pointed out, LMG1205 is a high current, high speed device. The app note is meant for more general purpose devices.

    We ask our vendors to use 2 oz copper on our boards.
  • 0 in reply to Don Dapkus
    Intellectual 960 points

    Hi Don, glad to hear that 2oz copper is workable. I see in the fab notes for LMG1205HBEVM that 2oz refers to finished thickness, which helps.

    If the LMG1205 is an exceptional case, then does it have a different recommended footprint from what's specified in AN-1112? The datasheet does not indicate a footprint, and I don't have the appropriate software to view the CAD files for the LMG1205HBEVM in order to inspect it precisely.

    AN-1112 also states:

    "The NSMD configuration is preferred due to its tighter control of the copper etch process and a
    reduction in the stress concentration points on the PCB side compared to SMD configuration."

    I don't see soldermask registration/expansion specified in the pcb fab notes for LMG1205HBEVM. Also doesn't specify LDI or LPI process. If LDI is used, would SMD pads be preferable? Not sure about the "stress concentration points" though...

    Regards,

    Mike

  • 0 in reply to Mike Twieg
    TI__Genius 12990 points

    HI Mike,

    Im an apps eng with this device and also work with Don.

    Check out page 23 of the LMG1205 datasheet for the footprint or land pattern dimensions.

    where are the PCB fab notes you are referring to?

    thanks,

  • 0
    Intellectual 960 points
    Hi Jeff, thanks for the replies.
    Right, forgot that there is a drawing in the datasheet, what I should have asked is whether it depicts the copper pads or soldermask openings. Now I see that it's the copper, for an NSMD footprint.

    The fab notes I'm referring to are in the design files for the LMG1205HBEVM (SV601338E1_FabNotes/pdf).

    I'll try to stick close to the EVM layout. However i think I'll have to shrink the mask openings a bit to get sufficient soldermask webbing (looks like <4mil in the design files).