• State TI Thinks Resolved
  • Locked Locked
  • Replies 15 replies
  • Answers 1 answer
  • Subscribers 34 subscribers
  • Views 3037 views
  • Users 0 members are here
Support feedback
Options
Options
Similar topics

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.

TMP007 Layout and Assembly Guide issues

Bill Norton
Prodigy 170 points
Other Parts Discussed in Thread: TMP007

Figure 24 shows the small-footprint layout modified by adding 10mil per side for shield mounting.

The 3.25mm dimension shown is inconsistent with the small-footprint layout in Figure 17.  That shows the copper area being 130mil wide, which is already 3.3mm.

Which is correct?  Should the copper area width be increased to 3.3mm + (2 x .25mm)?

Does the 200mil dimension in Figure 17 expand by .5mm to maintain the copper-free gap size?

Whichever is correct, to the same adjustments apply directly to the large-footprint layout, or would it be a proportional adjustment?  What about shield adjustments for the Laser Cut Micro Footprint?

The guide doesn't spell out whether the small copper fill in the center of the footprint should have soldermask over it.

  • 0
    TI__Intellectual 1385 points

    Hello Bill,

    I will forward this on to have someone look into this and assist you.

    Regards,

    Sensing Applications

    Jamieson Wardall

  • 0
    TI__Intellectual 1811 points

    Hello Bill,

     Essentially the two patterns are the same.  One is .127 and one is .130 it probably just got changed in the conversion to metric. The real modification is to suck the vias in and make them smaller, so that the lids will not short the vias. The lids that we have in house and that have been tested have a wall thickness of .008”.  The outside measurement of the lid is about .125”.  We were trying to give the lid room on each side to reflow nicely onto the pad, by leaving a .010 mil opening in the ground plane.

     Regarding the micro footprint:

    The micro footprint is not intended to be used with a lid.  It is designed for customers with space concerns and adding the lid adds to the overall footprint.

     Regarding the center copper fill:

    It should and I’ll look into getting that changed.

    Regards,

    Tommy Santoyo

    Sensing Applications

     

  • 0 in reply to Tommy Santoyo
    Prodigy 225 points

    I'm looking through the TMP007 datasheet and the SBOU143 layout guide, and I can't seem to find the pad size for the pins. 

    What's the pad size here? Thanks!

  • 0 in reply to tvich11
    TI__Intellectual 1811 points

    Hello,

         On our internal boards we use a 12mil pad.  The ball is a 15mil solder ball.  I looked through the documentation and couldn't find the information I will get this added to the documentation.

    Regards,

    Tommy Santoyo

    Sensing Applications

  • 0 in reply to Tommy Santoyo
    Prodigy 170 points

    The TMP007 datasheet mechanical section seems to show metric ball diameter:

  • 0 in reply to Bill Norton
    Prodigy 225 points

    Bill, thanks for pointing that out. While this shows the ball diameter, I still need to know the recommended landing pad size on the PCB. If you know how I can extrapolate that data from the ball size on the package please let me know!

    EDIT: Just read Tommy's post. Thanks Tommy!

  • 0 in reply to tvich11
    Prodigy 170 points

    So far I've been using the 10.8mil (.274mm) size I found in the gerber files for the TMP006EVM PCB.

    Haven't remembered where I downloaded those files though.

  • 0 in reply to Tommy Santoyo
    Prodigy 170 points

    Do you have a large footprint modified for a cover, or is the small footprint the only one suitable for cover mounting?

    On Figure 24 there are no via spacing dimensions similar to the 60mil dimension in Figure 10.

    When you say the vias were sucked in and made smaller, where did they end up and how big are they afterward?

  • 0 in reply to Bill Norton
    TI__Intellectual 1811 points

    Bill,

    The covers are not exclusive to the small footprint.  I have boards that I have created that have a cover over a 200mil footprint, that work fine.  The main purpose of the vias is to increase the thermal resistance between the board and the footprint, and to effectively slow down the transfer of heat from the board to the device.  The purpose of the cover, If it is well soldered to the ground plane, takes on the temp of the die or Ltmp. The IR sensor does not see the cover just what comes through the hole in the lid, effectively reducing the field of view.  

    The 8 vias surrounding the footprint on the small layout are .045in apart.  Keep in mind that we did this to reduce the footprint to as small as  we could to satisfiy board space concerns.  A little bigger or smaller does not mean failure.. It is the general pattern that needs to be followed to create the thermal isolation. 

                                                                             

    Regards,

    Tommy Santoyo

  • 0 in reply to Tommy Santoyo
    Prodigy 170 points

    Can you share a layout similar to Figure 10 for a large footprint modified for a cover?

    I have a prototype built with the large footprint, but it will need a cover.

    It looks like it would be simplest to expand the 180mil square by 10mil per side to mount the cover.  But that would reduce the thermal gap from 60mil wide to 50mil.  Would that harm the thermal design, requiring the 300mil dimension to be increased to 320mil?

  • 0 in reply to Bill Norton
    Prodigy 170 points

    Here's my attempt at modifying the large footprint from the TMP007 Layout And Assembly Guide to add a cover.

    The inner copper region grows by 10mil each side, reducing the copper gap to 50mil on each side.

    I kept the via positions and sizes from Figure 10 (30mil pad, 15mil hole, 60mil grid), and added

    two more of the same size for cover locator pegs, located 5mil inside the new outer edge of the copper region.


    Should I be concerned that the smaller copper gap and added vias will upset the board area's thermal performance?

  • 0 in reply to Bill Norton
    TI__Intellectual 1811 points
    I'm currently looking through my old files. I will put together a .ppt that shows the layout I used for my large lid. The gap at 50mils is fine. I think the larger the better, but 50 will be fine.
  • 0 in reply to Tommy Santoyo
    Prodigy 110 points
    Hi Tommy,

    I have a related question about the center copper fill's solder mask. Do you know if the color of the solder mask could affect the expected performance of a TMP007 device. I'm wondering if TI's characterizations were done with a particular solder mask color?

    Thanks,
  • 0 in reply to onechil
    TI__Intellectual 1811 points
    Our characterizations were done with green solder mask. I've had several conversations lately about leaving the center copper fill uncovered and plated with gold. Theoretically this would be better than solder mask. Solder mask emissivity is .8 gold plated copper is .0024. Hope this helps.
    Regards,Tommy Santoyo
  • 0 in reply to Tommy Santoyo
    Prodigy 110 points
    Yes it does, thanks for the feedback!