PCB Thermal Relief

Go To Last Post
18 posts / 0 new
Author
Message
#1
  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

Hi All

 

I am going to be updating a PCB, and would like review the thermal relief especially on connectors. 

 

Till now i have always use "Direct Connect" on my rules which makes a pin on a connector or a component pad connector directly onto copper pour such as GND or VCC.  And example is shown below. RED is GND and Blue is VCC.

 

I have not experience much issues on SMD components,but find it difficult when soldering connectors. 

 

This would mean, we would need to add a thermal relief. but what should ideal width be? Should it be 0.2mm or much higher such as 0.5mm?

 

Is it recommended have have thermal relief on SMD components? 

 

 

Thanks

Regards

DJ

Last Edited: Fri. Nov 13, 2020 - 03:05 PM
  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

Yes, I too find thermal relief on connectors helpful, but I have always taken what the default relief pattern was on the pcb cad software, and not had any problems, but if it is a high current(you decide what is high) then it may matter to you.  So far I have not had any issues needing thermal relief with SMD parts, but let your board assembly house be your guide. 

 

Jim

 

 

(Possum Lodge oath) Quando omni flunkus, moritati.

"I thought growing old would take longer"

 

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

It my be influenced by your build...if the entire board is heated up to melting temp, then  everything will melt.  ...if you are hand soldering something, then lack of thermal relief may mean it is hard to reliably hand solder a connector pin (or dig pout the big iron).

 

It get dicier when the copper is to be specifically used as a heatsink...max conduction is best for heatsinking, but works against hand soldering.

 

Aside from thermal relief...your #2 pin has no need for surrounding copper to be anywhere nearly that close to the pin...what purpose would it serve other than to make a great way to enable creating a solder short? Give yourself lots of elbow room & avoid a headache 20 mils, 30 mils, you have the space.  Solder mask is wonderful, but don't bet the farm on it, especially if you don't have to.    Do you want to spend hours finding that there is an intermittent short right where Fred swapped out a broken connector? 

When in the dark remember-the future looks brighter than ever.   I look forward to being able to predict the future!

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

Hi Jim

 

I am doing the PCB in house. SMD are being done using a hot oven and connectors are being done manually. Next board i am looking to see if i can use SMD versions.

 

But when it comes to thermal relief and high current , most of the connectors are low connectors e.g. membrane keypad connectors and JTAG connectors.

 

The connector with most current, will have to be the battery connector.

 

Unfortunately my software is an older version, where i need specify the thickness of track. I presume i can calculate the minimum thickness a track should be and use that, even though that pad would have 4 tracks.

 

Do you use thermal relief on smd components?

 

 

Thanks

Regards

DJ

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

avrcandies wrote:

It my be influenced by your build...if the entire board is heated up to melting temp, then  everything will melt.  ...if you are hand soldering something, then lack of thermal relief may mean it is hard to reliably hand solder a connector pin (or dig pout the big iron).

 

It get dicier when the copper is to be specifically used as a heatsink...max conduction is best for heatsinking, but works against hand soldering.

 

Aside from thermal relief...your #2 pin has no need for surrounding copper to be anywhere nearly that close to the pin...what purpose would it serve other than to make a great way to enable creating a solder short? Give yourself lots of elbow room & avoid a headache 20 mils, 30 mils, you have the space.  Solder mask is wonderful, but don't bet the farm on it, especially if you don't have to.    Do you want to spend hours finding that there is an intermittent short right where Fred swapped out a broken connector? 

 

Thats a good point. The spacing between two tracks was set to 0.15, but it seems that rule was also applied to all my copper pours, i will make a change and change this to 0.5-0.75mm.

Thanks

Regards

DJ

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

See this...

 

Executive summary - they can be a lot narrower than you'd think.

Attachment(s): 

#1 Hardware Problem? https://www.avrfreaks.net/forum/...

#2 Hardware Problem? Read AVR042.

#3 All grounds are not created equal

#4 Have you proved your chip is running at xxMHz?

#5 "If you think you need floating point to solve the problem then you don't understand the problem. If you really do need floating point then you have a problem you do not understand."

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

djoshi wrote:
Do you use thermal relief on smd components?

Only if I'm hand soldering and the part does not need that pin as a thermal pin, then yes.

When I'm doing hand soldering of smd parts, I normally apply solder to the pads with an iron, then use hot air to set the part in place.

 

Jim

 

 

(Possum Lodge oath) Quando omni flunkus, moritati.

"I thought growing old would take longer"

 

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

Ok, will start adjusting my PCB

Thanks

Regards

DJ

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

djoshi wrote:
Unfortunately my software is an older version, where i need specify the thickness of track

And no thermal reliefs in the standard/your pad library ?

 

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

No, i have to make my own rules,i don't think i can set this in my component library. 

Thanks

Regards

DJ

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

I always use thermal relief on SMD pads that are on a copper pour. I  think that my old EAGLE did that automagically. I do know that it was NOT part of the component footprint.

 

Everything I do, these days, are low voltage, low current except for the switching loop in switch mode  power converters. There, I follow the  manufacturer's recommendations as tightly as possible. 

 

Jim

 

Until Black Lives Matter, we do not have "All Lives Matter"!

 

 

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

I am using Altium Designer, and you set thermal relief using there rules.

 

 

Thanks

Regards

DJ

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

ka7ehk wrote:

I always use thermal relief on SMD pads that are on a copper pour. I  think that my old EAGLE did that automagically. I do know that it was NOT part of the component footprint.

 

Everything I do, these days, are low voltage, low current except for the switching loop in switch mode  power converters. There, I follow the  manufacturer's recommendations as tightly as possible. 

 

Jim

 

Is that necessary is your component  is smd and will be going into oven or soldered using hot air?

Thanks

Regards

DJ

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

I always design for hand attachment plus automated. Thermal relief does not hinder oven or hot air, so that is what I do so that I can construct and modify protypes.

 

Questions: (1) do thermal reliefs add to your cost? And (2) does it hinder oven or hot air soldering?

 

Jim

 

Until Black Lives Matter, we do not have "All Lives Matter"!

 

 

Last Edited: Sun. Nov 15, 2020 - 07:21 AM
  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

Thermal relief does not hinder oven or hot air

I generally always use thermal relief, except if high heatsinking is needed (such as a SMT transistor or linear reg is going to get really hot).   Those will solder fine in the oven, though may be tougher for hand-soldering.  Of course any thermal relief is doing its job to isolate the component from the large copper heatsinking area.

When in the dark remember-the future looks brighter than ever.   I look forward to being able to predict the future!

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

Thermal reliefs may help with the possibility of tombstoning - one pad being hotter than the other can cause the component to stand up, ie 'tombstone'.

 

 

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0


djoshi wrote:
No, i have to make my own rules,i don't think i can set this in my component library. 

I can't imagine a professional (as opposed to hobbyist) PCB tool like Altium Designer would make this core feature especially difficult; so I tried to find an old version page about it:

 

It appears these are the defaults, you only need to make your own rules if this won't suffice.

 

https://www.altium.com/documentation/altium-designer/pcb-dlg-polygonconnectstylerule-framepolygon-connect-style-ad?version=17.1

 

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

Kartman wrote:

Thermal reliefs may help with the possibility of tombstoning - one pad being hotter than the other can cause the component to stand up, ie 'tombstone'.

 

Not experienced the tombstoning issue at the moment, but will try to add them to my updated design. I also use 0402, so i am not sure how much thermal relief can be done on them?

Thanks

Regards

DJ