LT3759 exposed Pad

Hi Nico,

I've seen people say all sorts of things about the way to deal with this but to be honest just placing vias in the pad and approving all the resulting DRC errors seems the simplest way forward to me and I have done it this way plenty of times without issue. The only problem is if you move the IC and vias the DRC approvals need to be done again.

When placing vias in the pad like this you do need to be careful of the drill size. If the via is too large then the solder will get wicked away from under the IC when it's reflowed. With more complicated boards you can use a combination if microvias and buried vias to eliminate the solder wicking away problem but for standard boards with just through vias then just make sure the drill size for this is small enough to reduce the risk.

I think usually they are expecting that these devices are placed on multi layer boards with a solid 0V plane which doubles as a heat sink to take the heat away into the surrounding board. With a 2-layer board you wont have as much heat dissipation from this method so you might need to keep an eye on the device temperature when getting your board up and running. Also be aware that when building boards like this then the manufacturer who is assembling your board needs to know there are heatsink structures on these thermal pads so they can adjust their temperature profiles to ensure enough heat gets into the board so the thermal pad reflows properly.

Best Regards,

Rachael

Hi Rachael ,

thanks for the reply.

I 've also immagined that this kind of IC requires a minimum 4 layers board in order to benefit from the exposed pad presence but since its the first time I needed an advice on this issue.

Reading this tutorial (http://www.ti.com/lit/an/slma002g/slma002g.pdf ) from texas (see also the attached image) it seems that in a 1 or 2 layer board I can use the top layer for heatSink problem.

In addition it confirms what you said about using the 4 or more board layers board and buried vias.

So if I decide to use the 2 layer approach I should create a copper polygon as big as possible (the red figure in the attched image)  but I cant understand where (in the package editor) or in the layout board!

Do you have any advice on how to realize this ?

Thanks again for the support!

Nico

Hi Nico,

So in the package editor as part of the library part you need to create the thermal pad the correct recommended size for the part, this will ensure the solderable area on the pad a) doesn't have solder resist and b) is the correct size so that when it reflows it centres the part correctly otherwise your part can end up moving off your pads and not sitting correctly. Usually these thermal pads are connected to your 0V rail in your system, it usually tells you in the datasheet if it's to be connected to the same 0V reference as the 0V pins. You should put a pin on your symbol to represent the thermal pad and connect it to your system 0V if this is indeed the case.

Then in the schematic you would draw a polygon on the top layer (assuming it placed on the top of the board) around the pad and extending along the board to wherever you wanted it to be. You then name this polygon to 0V (or whatever you called your 0V reference) and it would connect to your thermal pad. You'll probably want to turn the thermal relief off (uncheck Thermals) in the polygon properties.

Let me know if you need any more help.

Best Regards,

Rachael

Ok Rachael,

Thanks again.

I usually draw a GND polygon on the TOP and BOTTOM layer after I have routed all the board that cover all the board dimension!

Do you think that they should be enough after I have properly added the exposed  pad (with  right dimensions as the datasheet says) in the package editor ?or do I have to make another GND polygon just for that device and another for the rest of the board on the top layer?

Sorry for the idiot question

Thanks  a lot again

Nico

Hi Nico,

So long as the polygon you add actually floods underneath the device and surrounds the thermal pad that would work. You'll need to make sure 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. 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. 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.

Best Regards,

Rachael

Thanks Rachael,

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

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

Check out tutorials from sparkfun.

Clem

More info on ti https://www.hackster.io/ti-launchpad/products

Hi and thanks again.

Now I have some points more clear.

So  if I decide to hand solder I should put the thermal structure through the all  board (like some people on you tube make) .

Which is the best way to do this in Eagle cad?

How can do this ? in the package editor or in the PCB  layout?

Could you please suggest an example?

Thanks a lot