What is thermal relief and what for?

thermal relief pcb

What is a thermal relief and wht is the need of a thermal relief?
Could I desing a PCB without them? What are problems associated with that?

pcb thermal relief

Thermal relief is a preventive action against overheating of electronic components, PCB vias etc..
Good example can be thermal relief pad around a via or around a pin of an IC.
As I said it is preventive action and in many cases you don't need to impose thermal relief practices, but as everything becomes smaller and smaller you have to think of despatching heat somehow..
Regards,
IanP

thermal relief

But the thermal reliefs are only for despatching heat in the soldering process or they are also usefull to dissipate heat when the IC is working?

thermal reliefs

Thermal reliefs on a PCB are to make it easier to solder and desolder thru-hole components when you have a circuit board with internal planes, large poured planes, or wide conducting traces. Without the relief patterns on copper planes (or wide traces), the planes (or traces) act as a heat sink drawing much of the heat away from the lead you are trying to solder or desolder. The result could be a cold solder joint, or the need to apply excess heat while soldering. Often it is impossible to desolder a component without damaging the board if that component was placed without thermal reliefs on the large connected copper areas.

Section 9.1.3 of IPC-2221 "Generic Standard on Printed Board Design" says:

QUOTE

9.1.3 Thermal Relief in Conductor Planes - Thermal relief is only required for holes that are subject to soldering in large conductor areas (ground planes, voltage planes, thermal planes, etc). Relief is required to reduce soldering dwell time by providing thermal resistance during the soldering process.

These type connections SHALL be relieved in a manner similar to that shown in Figure 9-4. The relationship between the hole size, land and web area is critical. See the sectional standards for more detailed information.

UNQUOTE

thermal relief pads

For a few examples of not having thermal relief:

On SMT components, if one side is connected to the groundplane, completely covering the pad and the other side is connected to a thin signal track.
While the component I.E. resistor/capacitor etc is going through the reflow oven, the side that has the groundplane connected to it will cool down much faster than the single trace side as there is more copper to dissipate the heat.
Then it tombstones/stands on end, or moves location & does not centre correctly.

A PTH component, similar connections. The groundplaned end will take much more heat to solder and bad joint may occur.
Soldering irons would have to be held against the joint for longer, possibly passing more heat through the device & harming it.

Also if it's a factory, the assemblers get used to a particular time per joint & if they have to spent longer on particular joints they whinge like heck & often do not solder them well.

thermal relief via

A wagon wheel-shaped relief pad etched in the copper of a ground plain around a through hole. It connects to the plane through one or more narrow track across an opening in the plane, rather than connecting directly to the plane, so that heat transfer to the plane is minimized during soldering.

Design can also be done without thermal reliefs if all the pads are made full thermal (i.e fully connnected to the planes)

pcb thermal pad

A wheel shaped thermal relief pads are strongly recommended especially on prototype boards for thru-hole components connected to the inner or outer plane signals. (gnd, power or other) Otherwise replacing the components without destroying the pins or the pcb thru-hole pads become impossible without using professional resolder equipments.
Generaly the PCB-design tools generate automatic thermal-pad or via insertion for the plane connetions.

what is thermal relief

Hi.. could anyone help me on how to design thermal relief for through hole padstack? thanks very much

padstack thermal relief

Thermal pads are used to make the soldering easier.A pad or via that is directly connected to plane represents the very efficent heat sink when trying to solder a connection.

Added after 3 minutes:

By reducing the amount of copper connectecd to the pad or via,you make it easier to heat the joint for soldering or unsoldering.

For large holes, 2 spoke connection is better, because more heat needed to solder these pads..

HI,
as i m new to pcb design and layout..can you clarify some doubts..

1.where/why do we use thermal relief pads.
2.do we use it for both thru-hole components as well as smd components
3.do we use thermal relief pads for both power as well as signal lines
4.do we use it for tracks as well as planes
5.what is tumbeffect
6.do we do thermal relief pads for vias also.i feel its not necessary for vias because we dont solder any component on that.


thanks in advance

IMO It is not necessary to thermally relive a via.

As you dont solder to it then the only thing your doing is making the connection worse.

On SMT components, if one side is connected to the groundplane, completely covering the pad and the other side is connected to a thin signal track.
While the component I.E. resistor/capacitor etc is going through the reflow oven, the side that has the groundplane connected to it will cool down much faster than the single trace side as there is more copper to dissipate the heat.
Then it tombstones/stands on end, or moves location & does not centre correctly.


very good suggs.....kept it up..

thank you for your answer...

can you tell any good book or reference to get all these basic things about pcb design and layout.I couldnt get any good material in google.

what is the dimensions we take for drill in a tru-hole component.as well as thrmal relief pad and anti pad dimensions


thanks in advance....

Added after 31 minutes:

Hi,
can anybody clear my doubts.i m new to allegro tool as well as pcb layout.

here in allegro for thermal pads there is no option like 'strip width','inner diameter','outer diameter'.it has only width,height,offset X,offset Y,geometry.
if i take geometry as circle and width 1.1mm and height 1.1mm its giving me a bigger pad than a regular pad.
why its given like this.how it is differ from thermal relief pad used for power supply.


thank you in advance.....

A. Normally If landpattern is provided in datasheet then you can take drill size as provided in the landpattern,otherwise as per IPC you can have a

Finished hole size (FHS) = Max Lead Diameter (provided in datasheet) + 10mils.
Anti Pad = FHS + 30 Mils
and for thermal - Inner Dia=Pad Diameter
Outer Dia=Inner Dia +20 mils


B.Thermals have to be created before you assign it for a pad.

To create a thermal you can go to FILE -> NEW -> provide a name for the thermal.

select Drawing type as flash symbol. click on OK.

Now check the user units - whether u need in mils or mm.

Go to add -> Flash.

Here u will get the window.where you need to enter the inner /outer dia,spoke width etc.

After you save this, assign this as flash for your pad.

One thing I didn't see mentioned is the fact that most of the time, you do not need a thermal for your vias, any connected to a plane can simply be flooded over.

As others have said, thermals are only really necessary for plane connections for TH components, and SMT parts when tied to a surface plane.