Hello. I have repeatedly suffered from strange difficulties on an even ground in Kiсad. And so I have a few questions.
1:
Tell me how to design the PCB to make the elements are installed as the tracks at a certain distance and were not put closer. Otherwise, you have to constantly move the body of different elements so that they are all at equal distances from each other.
2:
Why when searching and assigning seats for a separate element there is no built-in browser of the type of this seat. A browser can run in a separate window (View selected footprint), which is terribly indescribably inconvenient.
However, in PCBnew when you select to add a footprint on PCB and click on the button - select the browser, on the window that appears, on the contrary, everything is there and view and select from the library various footprints
3:
How and where can I choose the type and view of thermalload for the contact pad? However, even in such a simple PCBeditor as a Sprint Layout, everything changes elementarily.
I am not really certain what you mean. In general kicad has many options on how to assign footprints and all of them have a way to show a preview (which i assume is what you are looking for.)
More details see: How can i assign a footprint to a symbol?
In your screenshot you measure relative to what i assume is the courtyard outline. You do not measure against the body size of the component! (The body is smaller than the bounding box taken up by the pads for such devices.)
The courtyard area is already what should be used to ensure you have clearance between parts (The official footprints use IPC [industrial standard] nominal density rules here. These rules specify 0.25mm clearance to both pads and body.)
No, this is not what is needed. Just in your link in a separate window shows how to see footprint (section Activate previews in cvpcb), and this is extremely inconvenient. I need everything in one window as when adding a new footprint in pcbnew (as last screenshot)
It does not matter how to measure. I just need to set a strict distance between the components on the board. So that the distance between the elements on the PCB, during installation and positioning, could not be less than the specified. Just as the minimum clearance is specified in the design rules for printed conductors or in other words for flat tracks.
That is what the courtyard layer is for. Draw the area you need for installing a particular component onto it and kicad will complain if you place another component too close.
If you read the full tutorial you will notice that there are tools that allow for exactly that. And you can easily simulate the one window behavior even for cvpcb. You know your window manager allows for having multiple windows visible at once. (Will of course reduce the space available for cvpcb but that would happen even if it is a single window.)
I do not need an area for a specific component. I need a rule for all components and for any components. Just as rules are created for all printed conductors.
p.s. …give me please a link to read about courtyard
I just had a peek in the KiCad documentation because of your courtyard question: http://docs.kicad.org/
Unfortunately there is not much written about courtyards in the KiCad documentation.
From what I understand the Courtyard is the area of the component, with extra room around it, so it can be placed on the PCB by automated equipment. Some work with suchtion cups on the top of components to place them on the PCB, but for other components there may be grabbers on the side of the componets, which also needs some clearance.
If the courtyards are designed well, then the courtyards of the components can be placed touching each other, but not overlapping. In this KiCad handles them differently from the clearance between tracks.
When you do a DRC check in Pcbnew, it can generate errors for overlapping courtyards. To get a better Idea of the pre-defined courtyard size compared to the components themself, move a few components in such a way that the courtyards are just touching, and then view your PCB in the 3D viewer.
Often though, the courtyard is not the limiting factor. quite often you need to space the components further apart to have enough room to lay the tracks.
Courtyard – The smallest rectangular area that provides a
minimum electrical and mechanical clearance (courtyard
excess) around the combined component body and land
pattern boundaries.
So exactly what @TViT needs. But as this standard defines a fixed courtyard for a given density level there simply is no need to have this configurable dynamically at design time. (Having a well made footprint generator that has a setting for this is sufficient. Which is why i pointed to our generator scripts.)
Of course a more dynamic way of defining this might allow for even more usecases to be captured but i would assume these to be of low priority. (I suggest to make a feature request on launchpad for this. But make a well reasoned usecase description that shows where the standard way of using a static footprint defined courtyard does not suffice.)
For now the best advice is to modify the courtyard of your personal footprints such that they define the courtyard area with the clearances you desire. (But remember if you define the clearance the same for all parts then you only need to have half the clearance designed in every component as courtyard is checked against courtyard of nearby footprints.)
And kicad specifics can be found in both the KLC and the forum FAQ:
