Actions
Forum Thread Details
  • State Suggested Answer
  • Replies 14 replies
  • Answers 1 answer
  • Subscribers 180 subscribers
  • Views 1935 views
  • Users 0 members are here
Related

LT3759 exposed Pad

nikoly

I'm using a 2 Layer Board in Eagle .

The datasheet gives some info about the layout, advising me to add some  vias inside that Pad for heatsink problems.

I have opened Eagle tutorial "ti-launchpad" where there are  2 IC with Pads and vias on them (how in the image)p .image

Watching the DRC I have some overlap errors.

I can follow that way in order to design my board but I wonder if it's the right way to do this or not !

I have also seen someone to put arrays of pads instead of vias in order to get this!

 

Hope you can put me in the right direction!

Thanks a lot

Nico

Parents
  • 0

    Thanks Rachael,

    I have to admit I have a lot of Gaps in PCB designing image Sorry

     

    When you say :

    other component placement and/or routing hasn't isolated that area of your board from GND thereby stopping it flooding the area under the part with your GND fill

     

    I think you refer to the fact that there should not be any component wich prevent me to have 100% GND around the exposed Pad?

     

    One thing you will probably find doing this though is that you won't want to turn thermal relief off for the entire GND polygon for the board or you might end up with a board that is really difficult to build

     

     

    Do I have to put  thermals on on my Main GND polygon (top and bottom) in order to easy solder the board ?

     

    So you might need to put another small polygon underneath with the thermal relief turned off to surround the area around the pad plus a little more to cover up the thermal relief on the main GND polygon for that pad.

     

    Should I have to put 3 polygosn ? one around the exposed pad with thermals reliefs off , one little more with thermals relief off to cover the main thermals relief of the Main poligon and one Main Polygon with thermals relief on in order to solder without difficoult the whole boards?

     

    Sorry If I didnt understand !

     

    Hope you can help

     

    Nico

Reply
  • 0

    Thanks Rachael,

    I have to admit I have a lot of Gaps in PCB designing image Sorry

     

    When you say :

    other component placement and/or routing hasn't isolated that area of your board from GND thereby stopping it flooding the area under the part with your GND fill

     

    I think you refer to the fact that there should not be any component wich prevent me to have 100% GND around the exposed Pad?

     

    One thing you will probably find doing this though is that you won't want to turn thermal relief off for the entire GND polygon for the board or you might end up with a board that is really difficult to build

     

     

    Do I have to put  thermals on on my Main GND polygon (top and bottom) in order to easy solder the board ?

     

    So you might need to put another small polygon underneath with the thermal relief turned off to surround the area around the pad plus a little more to cover up the thermal relief on the main GND polygon for that pad.

     

    Should I have to put 3 polygosn ? one around the exposed pad with thermals reliefs off , one little more with thermals relief off to cover the main thermals relief of the Main poligon and one Main Polygon with thermals relief on in order to solder without difficoult the whole boards?

     

    Sorry If I didnt understand !

     

    Hope you can help

     

    Nico

Children
  • 0 in reply to nikoly

    Hi Nico,

     

    Okay I will try and answer your queries:

     

    nikk kik wrote:

     

    other component placement and/or routing hasn't isolated that area of your board from GND thereby stopping it flooding the area under the part with your GND fill

     

    I think you refer to the fact that there should not be any component wich prevent me to have 100% GND around the exposed Pad?

    Yes so basically the polygon has to flood fill the board but it can't get through gaps which would cause it to violate design rules. So if there is no path to flood the GND polygon underneath the IC it wont fill.

     

    nikk kik wrote:

     

    One thing you will probably find doing this though is that you won't want to turn thermal relief off for the entire GND polygon for the board or you might end up with a board that is really difficult to build

     

    Do I have to put  thermals on on my Main GND polygon (top and bottom) in order to easy solder the board ?

    You don't HAVE to, it very much depends on what other components you have on there and how the boards are to be assembled. If you have lots of through hole pins with GND connections and you are hand soldering then not having the thermal relief might make your life a bit harder. If it's being professionally built then the PCB assembly house will have a pre-heat phase in their reflow profile to bring the core board temperature up so the reflow phase works more quickly and exposure to high temperatures can be minimized.

     

    nikk kik wrote:

     

    So you might need to put another small polygon underneath with the thermal relief turned off to surround the area around the pad plus a little more to cover up the thermal relief on the main GND polygon for that pad.

     

    Should I have to put 3 polygosn ? one around the exposed pad with thermals reliefs off , one little more with thermals relief off to cover the main thermals relief of the Main poligon and one Main Polygon with thermals relief on in order to solder without difficoult the whole boards?

    No you just need one extra polygon underneath the part surrounding the thermal pad, large enough to cover the thermal relief around the pad. If you aren't worried about solderability on the main GND polygon you can dispense with this and just turn thermal relief off on that.

     

    If you are hand soldering you might want to put the thermal structure through the board. I've seen a technique (although not used it myself as all my boards get built by a contract manufacturer) whereby you can apply heat to the thermal plane on the underside and the heat transfers through the thermal vias and reflows the solder paste on the thermal pad underneath the part.

     

    Best Regards,

     

    Rachael