I hereby certify that I am not simply asking someone else to design a footprint for me.
This is an auto-generated message that is in place on the “footprints” section of the KiCad.info forum. If I remove it and ask for a footprint to be designed anyway, I understand that I will be subject to forum members telling me to go design my own footprint or referring me to a 3rd party footprint site.
Hello, I was designing a pcb and trying to fill a specific area using the add filled zones function.
The area I want to fill is the area where 12V 2.6A flows.
“Thermal relief” belongs to basics of PCB design. I you try to hand solder, the heat will be very rapidly spread to the surrounding copper and the place which should heat (the pad and the component leg) stay too cold. Therefore solid connections are replaced with thinner traces. This is very usual for THT components: there’s a round THT pad, around it there’s empty space and the pad is connected to surrounding copper area with 4 thermal reliefs. Now the heat stays in the pad and the leg when you solder it.
If soldering is done in an oven it may be better to use solid connection, but it depends on the situation.
As eelik wrote. “Thermal relief” is a standardized term with a specific meaning.
From your screenshot:
This has only one “thermal spoke” connected to your pad. If your pad is surrounded on all sides by the copper zone, then it will have 4 of those spokes and the way it works will be more obvious. Just try it out. You can always exit KiCad without saving, and then load the PCB again if you mess up.
The what has been answer (ie thermal relief is necking of copper to provide thermal isolation during soldering) but what can be done?
The copper shape in question is attempting to link four components ( three SMT, one THT). A solid fill fully connects all nodes but thermal-relief produces the needed spokes but also results in an unconnected pads.
The issue can be improved by using the thermal relief settings
THERMAL CLEARANCE - gap between the pad and the fill
THERMAL SPOKE WIDTH - how wide a spoke is.
By changing these settings an improved connectivity can be realised. You might need to increase the actual size/shape of the zone to help with connectivitity
NOTE: Kicad only permits a maximum of 4 spokes and at 90deg (sometimes it is useful to have them placed on a 45deg rotation)
Here is a screenshot from a design of mine where I have a D2Pak resistor as part of a damping network. You will notice that pin1 only has 3 spokes because of another constraint (edge of the zone) overrides the ability to add the 4th
By enlarging the zone the 4th spoke can be added - I couldn’t do this as there is creepage considerations… I only need to dampen out a transmission line so the current is low.
I don’t know what T.T means.
I suggest to set ‘Thermal clearance’ zone parameter smaller, and ‘Thermal spoke width’ bigger then you have.
And you can make your zone bigger to have more of it around 7,8 pads.
On round pads a work around is done by rotating the pad, the you can have the spoke in whatever direction that you like, however still 90° spaced from each other.
I do not like to use thermal relief connections. My solid connections do make soldering more difficult (more heat is required.) The most important reason for solid connections is for cooling (“heatsinking”) of surface mounted power (semiconductors and maybe some resistors.) Cooling components in this way can be very useful and is often needed.
Use where applicable.
Some 15 to 20 years ago I worked in a company that made and serviced security cameras. The PCB’s were probably 6, maybe 8 layers and on both sides filled with lots of chicken fodder. Only the image sensor and some connectors were THT, and one of the GND pins of the sensor was connected without a thermal relief to some inner zone, an that made replacement for that sensor very difficult, while the image sensor itself had no problems with temperature whatsoever.
On the other side of the spectrum I’ve seen the tab of an LM1117 in the middle of a substantial copper heatsink, but connected with thermal reliefs.
I think @eelik has given you a fairly comprehensive summary of how thermal reliefs work and how they compare to solid connections. The choice may be influenced by the thermal properties of the components, whether you are using SMD or THT technology, the type of production process (e.g. wave vs reflow vs hand soldered), RF considerations etc. There are other manufacturing issues, for instance, particularly when using small components, if the thermal properties of the pad connections on a component are very dissimilar the surface tension in the molten solder can be different at opposite ends of the component, this can lead to tombstoning.
This is a matter of PCB design and not really KiCad specific. IPC2221A provides some more info.
My first reaction was that maybe LT1117 is correct and not LM1117. But to find components I usually like to go to Digikey or Mouser so I am finding real components and not counterfeit or somebody selling datasheets. (really). I think that Bob Widlar at National first invented and made the LM117, then LT made the LT1117, then National copied that and called it the LM1117. I did find the LM1117:
LM or LT, maybe it was an AMS1117 but it was a SOT223 package. It’s all the same difference as from der.ule’s picture. It was to be expected that more then one people in this world would make such a mistake.
I am not completely sure who is doing what, but from the picture I see:
LM1117-DTX. That is a TO-252 according to the TI datasheet. In case anyone does not know, TI bought National Semiconductor some years back. Originally National Semiconductor ICs were generally identified with part types beginning with “LM”.
I have trouble keeping TO package designations straight but the photo does look like a Dpak. I think is that is “the same” as TO-252. Package designations drive me nuts.
Indeed I see that the heatsinking of REG2 has been largely defeated by a thermal relief connection between the tab of REG2 and most of the copper zone.
Perhaps these statements will help: (all refer to a pad connected to a ground plane)
Copper conducts heat. By conducting I mean allows heat to flow from one area to another, the more copper area the easier it is for heat to move to the various places on the board. Heat will stop flowing when all areas are the same temperature.
Thermal reliefs are only an aid for hand soldering (either initial assembly or repair). They limit the amount of heat that flows from the pad to the ground plane. Thus allowing a hand soldering iron to heat the component and pad quickly for a good solder joint.
Thermal reliefs are bad for cooling hot components because they (as above) limit the heat that can be spread around the ground plane, reducing the cooling effect of the copper area.
When to use:
When you have small components that generate no significant heat.
When not to use:
When you have a power device that will generate heat and the only method of cooling is convection and spreading the heat over a large area (of the ground plane)
Often power semiconductors with large heat spreading ground plane must be soldered by an alternate method. I use a thick aluminum block heated to ~350°F. I hold the board above this block for 60 seconds then drop in onto the block. I solder it quickly then move the board away from the block by about 1/4 inch for a minute, then remove it from the heat.
Others use a convection oven. However this method requires the use of solder paste.
