Courtyard for PCB connectors

Hi all guys,

I want to make footprints for audio 3.5mm stereo connector (SMT) and for USB A connector to meet IPC 7351 standard. However, after reading the standard I was not able to find how to set the courtyard for such components.
Additionally, I was able to find an explanation inside the IPC 7351 about the courtyard which follows component contour. Is it true that is the part of the 7351C stanard?

Cheers and thanx!

IPC-7351 : Generic requirements for Surface Mount Design and Land Pattern Standard.

The IPC-7351 are requirement for land patterns, based on the dimension of the part. In general a courtyard will include all the items that makes the land pattern for a given component. At our institute we use two courtyards, one courtyard has the same dimensions as the maximal physical component outline and also has the maximum height defined.
The second courtyard includes everything that makes the total land pattern and has a height of zero. This (larger) courtyard is used in placement/DRC.

When creating components it is important to define some rules on how to build land patterns. (Library Spec) This is the only way to create/maintain a library of high quality. And remember, although not always as obvious as it should be, your library is the most important asset in Schematic/PCB design.

Thank you for your answer senilicus. Could yu please share what is the distance between some connector footprint and its (second, zero height) courtyard in your library? And why do you use this value?

My problem is I was not able to find any such information inside the IPC-7351. They are only providing tables with values for known packages ...

Traditionally the outline courtyards would be squares, rectangles, circles etc. as this was the easily generated shapes for the CAD software used.

However, this can often leave blank areas of the PCB that could have a component in, but doing this would leave "component to component" errors as you'd have one inside another.
I.e. when you have a connector that has a big rectangular placement courtyard however it has big spaces where you can fit other small components without problem.

So AIUI the IPC7351-C courtyards now reflect the true shape of the components, this allows greater placement choices/ability where you can utilize unused space - which is more of a premium now things have got smaller.

The courtyards are explained in IPC-7351B near the first 1/4 of the doc.

If making a component manually I would always make a placement outline, used to enable me to place the components - this follows the contours of the component and used to be 0.5mm from the pad edges (assuming the pads are the extent - if not the physical component edge), then when placed I would get 1.0mm between pads of adjacent components (or component to component) - this used to be the rule of thumb distance for best placement and soldering/thermal distance. (taken from an old Siemens guideline document - prior to IPC standards.)

Things have changed (a long time ago) and now the distance is a lot less - depending if you use the least, nominal or most spacing's and the manufacturing class recommended by the IPC standards.

I would also add manufacturing values into this courtyard if for instance it was a tall component so that thermal shadows were not affecting others although this would generally be with a secondary placement outline, I also place assembly outlines on an assembly layer for the assembly documentation, silkscreen outlines (where required) on the silkscreen layer.

The more thought that you put into the creation of your components, what outlines will be needed, what shape and spacing they need to take, what layers they go on and where and when they will be used - the better your component library will be, the more accurate, the more useful and the easier your job will be.
This is why we use standards whenever we can, they maintain accuracy and consistency.

When you manually make components you need to calculate and draw your outlines yourself, although for the majority of your components you can now use the Library Expert program (there is a free version available) where you simply specify the values to be used and it auto creates all the outlines for you, the pads etc. Export them to your CAD package type and import them into a library.

We use 0.25 mm clearance for the second placement outline from every item that is included. Have no idea where that value comes from. Used it for decades.

IPC-7351B is still the official standard I believe, C has yet to be approved by the IPC.

Talk about slow...

I think that the IPC-7351 is a great idea, my concern now is the constant changing really required or is the IPC being pushed in this direction by people who have a monetary interest in the standard changing... I also believe this is why it is getting unnecessarily complex, I keep seeing libraries with multiplke footprints for the same components such as SOT-23 (SOT95 etc) devices, there should only be 2 a nominal and a least.
Most basic SMD components have been here for years, what started out as a good idea is getting extremely complex and that is wrong, should always keep things simple, simple generally is more elegant.
At the end of the day the IPC-7351 is a guide so if you need to use placement outlines that follow a components contours... DO IT.