Continue to Site

Welcome to EDAboard.com

Welcome to our site! EDAboard.com is an international Electronics Discussion Forum focused on EDA software, circuits, schematics, books, theory, papers, asic, pld, 8051, DSP, Network, RF, Analog Design, PCB, Service Manuals... and a whole lot more! To participate you need to register. Registration is free. Click here to register now.

Register Log in

What isolation between LED tab and cathode/anode?

Status
Not open for further replies.
T

treez

Guest
Newbie level 1
LED footprint with pads smaller than the LEDs actual pads

We are making a footprint for the L1C1-RED1000000000 LED

LED Datasheet:
**broken link removed**

The recommended land pattern on page 27 of the datasheet shows the PCB pads being smaller than the actual LED’s own pads. (LEDs own pads shown on page 25)

-Presumably this is to stop the LED from sliding about when placed?
If I make the actual PCB pad 0.1mm bigger (in all directions) than the actual LED pad, then is this really going to be a disaster when the LEDs are placed?
 

Re: LED footprint with pads smaller than the LEDs actual pads

I have done these devices with the pads 1:1. Even though they show the pads smaller when these devices are put on a board they are connected with maximum copper for heat sinking purposes so with the recommended solder mask opening you effectively get a 1
;1 pad. So I use IPC-7351 standard and use a 1:1 pad with a 1:1 solder mask opening and get the same result.
 
  • Like
Reactions: treez

    T

    Points: 2
    Helpful Answer Positive Rating
Luxeon C color line LEDs
**broken link removed**

..do you know what is isolation from thermal TAB to cathode/anode? datasheet doesnt say....can we join TABS of different LEDs with the same copper pour?
 

Hi,

Datasheet - Mechanical Dimensions - show 0.30 mm +/- 0.05mm - 2x

Klaus
 

Thanks, but i mean is the tab electrically connected to either anode or cathode, and if not , what is the voltage isolation level from tab to cathode and anode?
Can tabs of different leds be connected together by copper pours?
 

The centre pin is an isolated thermal pad (page 25) so they can be connected together, I usually use a GND connection then I can add thermal via's down to a good solid ground plane (if there on a multilayer board). If its a single sided design with metal clad PCB I fasten it to one of the other pads just to increase the actual copper connected to the led.
 
  • Like
Reactions: treez

    T

    Points: 2
    Helpful Answer Positive Rating
I don't apply to do your design work and calculate the thermal impedances in detail, but it looks quite obvious that a copper area larger than the minimal 1.8 x 1.8 mm of the bare footprint will achieve better heat sinking, even on a 100 µ dielectric of thermal clad PCB. I calculate a thermal impedance of 45 K mm²/W or 11 K/W for a 2x2 mm copper area (putting in 2.2 W/m K dielectric thermal conductivity given in Bergquist datasheet).

Copper has about factor 180 higher thermal conductivity, at least a few mm surrounding copper pour make sense. At this point, an advantage of 70 µm copper against 35 µm comes into play if you are targeting for smallest possible LED over temperature.
 
  • Like
Reactions: treez

    T

    Points: 2
    Helpful Answer Positive Rating
I concur, 70um copper is far better at spreading the heat. I will try and find an example of some similar boards I have done...
 

I must admit i always like to have large thermal copper lands connected to SMD pads, but with our tiny LEDs, i fear doing it without thermal reliefing as the LEDs might not solder properly, if the exterior copper land draws heat out of the actual footprint area of the pad during soldering...therefore i thermal reliefed the connection of thermal copper lands to the LEDs as follows.....(attached)....maybe i could have gotten away without this?...
 

Attachments

  • LAYOUT___LED MCPCB.pdf
    115 KB · Views: 197

I must admit i always like to have large thermal copper lands connected to SMD pads, but with our tiny LEDs, i fear doing it without thermal reliefing as the LEDs might not solder properly, if the exterior copper land draws heat out of the actual footprint area of the pad during soldering...therefore i thermal reliefed the connection of thermal copper lands to the LEDs as follows.....(attached)....maybe i could have gotten away without this?...
Click to expand...
Doesn't sound well considered. The board will be soldered in reflow oven or an a hot plate, uniformly heating the whole board. Hand soldering or repair of thermal clad boards is hardly possible without preheating the board on a hot plate.
 

Thanks, do you think the attached modofication is better/acceptable?
Its 70um copper.
All the LED tabs are connected and there is no thermal reliefing because i assume this is never necessary for MCPCB since as you allude, all layers are heated to virtually the same temperature when being soldered in the machine?

I also assume that the LED's cathode and anode pads are not useful for connecting to thermal copper, since it is only the internal bond wires which connect to them, so hardly any heat will pass down these thin bond wires, and so therefore, little effort should be made to connect thermal copper pours to the LED's anode and cathode pads?...instead, the majority of the board area outside the LEDs should be assigned to thermal copper which connects to the LED thermal tab?
 

Attachments

  • LAYOUT__LED MCPCB.pdf
    107.3 KB · Views: 170
  • SCHEMATIC__LED MCPCB.pdf
    71.4 KB · Views: 153
Last edited by a moderator:

The layout is now as in the pdf in post #11. As you can see, there is a large single thermal copper pour connected to all the thermal tabs of each LED. This large copper pour is in fact floating. Should i tie it to some electrical node so as to stop it from floating up to some high potential, whereby it may then break over the isolation between tab and electrodes in the LEDs?

I note that our MCPCB is also actually floating, and i wonder if it is necessary to ground it with a ring terminal which gets screwed to the MCPCB, and then wire this terminal to ground?
 
Last edited by a moderator:

This question s related to the above...

If you have a component with pads which have just a 0.25mm gap between them, then there is the problem of getting a solder resist “slither” in between these pads. This is because solder resist placement tolerance is usually +/-0.75mm. So if the solder mask opening is extended to 0.075mm outside the pad edges, (so you can avoid getting solder resist on the pads) then that means that with the 0.25mm gap between the pads' copper, then your solder resist “slither” between the pads is just 0.1mm wide. …-No PCB manufacturer can reliably produce a 0.1mm wide “slither” of solder resist between adjacent pads…….
So in such a case what do you do?....
You can either reduce the solder mask opening, and make the solder resist “slither” wider, but risk solder resist going onto the edge area of the pads, or you can keep the solder mask opening where it is, and risk there being no solder resist being between the pads. Which one do you choose?
 

There might be different design rule specifications by your thermal clad PCB manufacturer. The numbers are however wrong as general rules. A typical solder resist specification for recent high density PCBs is 50 µm clearance and 100 µm minimal structure (bridge) width, resulting in 200 µm minimal copper pad clearance.
 
  • Like
Reactions: treez

    T

    Points: 2
    Helpful Answer Positive Rating
OK thanks,

But supposing the pads were so close that you had to choose between...

1...Not having any solder resist 'bridge' between the pads..
2...Having the solder resist "leak" over the edges of the pads.

.....which one of the above 2 would you choose?
 

Neither I would go to where I could get the job done properly, clearing shorts or having badly soldered pads due to solder mask intrusion is just not acceptable these days. Simple quality counts.
 
  • Like
Reactions: treez

    T

    Points: 2
    Helpful Answer Positive Rating
We had pads that were 0.25mm apart. We wanted to extend the solder mask 0.075mm outside these pads……because the PCB manufacturer told us that we would have to do this to guarantee not getting solder resist onto the pads. however, this would have meant a ‘solder_resist_bridge’ of width just 0.1mm between the pads……the PCB manufacturer told us that the minimum solder_resist_bridge that they could guarantee was 0.13mm….therefore, we actually went for a 0.15mm ‘solder_resist_bridge’ between the pads, and then obviously our solder mask was only 0.05mm wide of the pads…..this means that we will get solder resist onto the outer 25um part of our solder pads.
Do you think this is OK?
It seemed to us that the worst case scenario was not having a decent solder_resist_bridge between the pads.
 

Get a new manufacturer, that's what I would do, as stated the cost of any problems will cost more to fix than getting the boards right correctly.
 
  • Like
Reactions: treez

    T

    Points: 2
    Helpful Answer Positive Rating
Thanks, but to be honest, i would doubt that anybody could spray solder resist on to a PCB with accuracy better than 0.075mm. Also, with a solder_resist_bridge, i would again doubt any manufacturer coul dgaurantee making a continuous solder_resist_bridge of any less width than 0.13mm
 

Look up manufacturers capabilities... I have solder dams 0.1mm and smaller done all the time...
 

Status
Not open for further replies.

Similar threads

Part and Inventory Search

Welcome to EDABoard.com

Sponsor

Back
Top