LT3759 exposed Pad

Thnks a lot ,

this is my first smd project . I only  worked with pth components before.

Hope to have success with it in order to waste my money 

Best Regards

Nico

Hi Nico,

You're welcome, good luck with your design. If you need anything else let me know :-)

Best Regards,

Rachael

Ok Rachael .

Thanks for all your time and patience .

This is what i call a perfect support!

Nico

nikk kik wrote:

 

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

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

 

Hi Nico,

This is basically as we discussed initially, so you start by creating the package with the thermal pad defined correctly as per the datasheet, this ensures the solder mask and paste mask are defined correctly so it doesn't move to the wrong place when the solder paste underneath it reflows.

Then you have a couple of choices:

You could add additional polygons top and bottom side in the board and add the vias between them. Just name the polygons and vias the same as the net the thermal pad connect to which I think in your case will be GND.

Alternatively you could build the polygons and into the library part. This has the advantage that they'll appear automatically on all parts placed but the disadvantage is that you'll not be able to alter/remove them if they are in the way anywhere without editing the library part again. You then put the via's between the two in the board as previously or I think you could do it using correctly sized TH pads placed within the polygons. You'd need to ensure they were all connected to the same pin as the thermal pad. This method may throw up a bunch of DRC errors but I am not sure as I haven't tried it this way myself, I always just do all this in the board as I find it quite easy.

With either of these options it may be worth putting a small polygon on the bottom solder mask layer inside the bottom side heatsink polygon to leave a small area of copper exposed so your soldering iron makes a good thermal contact with the copper to help get the heat up through to reflow the thermal pad more quickly.

Best Regards,

Rachael

EDIT: Added comment about on bottom side solder mask.

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

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

Check out tutorials from sparkfun.

Clem

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

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,

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