I’m going to use this type of pluggable screw connector in my design. (I’ve changed my design and am not using the fixed screw terminal block I recently asked for anymore.) It has a pin pitch of 3.5 mm. They also suggest a through-hole diameter of 1.2 mm. Here’s a description:
I can’t find it in the library for the schematic or footprint or 3D model. Does somebody know what ID this one is listed under? This form of connectors seems to be more widespread and also available from other manufacturers. (I’ve seen it from Würth and Phoenix Contact.)
I wish there was a reverse picture search in KiCad that would find me the correct entries if I show it a photo of the physical thing I have.
This is for terminal blocks which are very different parts to what is shown in the link by @Anders_Wallin (A terminal block is a single part that connects to both the cable and PCB, what is shown in the link is a two part connector system that happens to have screw connections on the cable side)
@Rene_Poschl and @Anders_Wallin pointed you to some good resources. The unwritten foundation under both replies is that you should learn to draft footprints. Whether you create a footprint using a script, or modify a similar footprint, or draft it from scratch, it’s a skill that is at least useful - and, some would say, essential - if you do more than two or three boards per year.
This particular pluggable connector has two characteristics that are uncommon among footprints. The first is the “courtyard” area. Make sure you allow unobstructed space for the mating plug to mate and unmate. KiCAD footprints have layers dedicated to courtyards. The second item has to do with board edges. Depending on the design of the mating pluggable section, this connector may require placement at a particular location with respect to the board edge. Unfortunately, KiCAD footprints do not (yet) include information for the Edge.Cuts layer, so you’ll have to place this information on another (non-copper) layer and hope you remember to look at that layer while designing your board.
They can include it but this connector really should not. My reasoning is that if an edge cut is included then the drawn edge must be the only option where to place the edge. This connector has reasonable wiggle room of a few mm for where the edge can really be (source: The similar phoenix connectors were one of my first contributions because I used them in nearly every of my projects.)
I am also not convinced that including the cable side for the courtyard would be a good use of that layer. One places it at the board edge anyway and including the cable side in the footprint would limit the validity of the footprint (the cable side of connectors like this is available in a surprising number of very different versions.)
The Gold is of course from the pads, which apparently can not be turned off in the 3D viewer, but then again, the pads are the most important part of the Footprints.
KiCad is pretty amazing!
The MCV Rene suggested is the vertical variant of this connector and also in the same library.
A trick for searching in the footprint libraries is to type a partial name, “conn” will do for connector, a space and another search string, in this case “3.5” for the pitch of the connector. This narrows your search down significantly.
Be carefull with these connectors. They come in a pitch of 3.5mm and also with a pitch of 3.81mm, which are not interchangable.
The bigger variant has a similar annoyance. They come in a pitch of 5mm and 5.08mm and are also not interchangeble (for connectors with >4 or 5 contacts)
The remaining question is:
Are there too many connectors in KiCad libs, or did you not install the lib’s?
I have “just” the regular / normal lib’s which come with KiCad V5.
Wow, the “Connector_Phoenix_MC:PhoenixContact_MC_1,5_4-G-3.5_1x04_P3.50mm_Horizontal” footprint and corresponding 3D model looks like the right choice! Also the hole diameter has been set.
It would have been a lot of guesswork to create the footprint manually because I don’t have sufficient data on the geometry of the thing. Would have to measure it out from the device itself and derive some data. Also, the manufacturer can’t provide me any more data, I’ve asked them.
I think my problem is there are too many connectors (and in general too much everything). It’s appreciated to see the parts I need are there (most are), but I can’t find them in the sheer masses. The only thing I could browse through is footprints but I’m not sure if they’re what I’m looking for. 3D models are extremely hard to browse. Also, often I just don’t know the model number or manufacturer or product name (search terms) and then the category KiCad has organised that into. I have a default installation on Windows, with all the libraries that come with it, gigabytes large.
If there’s not a proper datasheet, you’ll need to buy and measure the part. Or better yet, throw it away and use one of the thousands of alternatives whose manufacturers release proper specifications.
I found the connecttor pretty quick in the library browser with the search term I mentioned in my previous post.
You can also have the Footprint browser and the 3D viewer open at the same time (next to each other, so don’t maximize the view). Then you can see the current selected footprint from the Footprint viewer in the 3D viewer, also just as in the screenshot I posted earlier. (There I made the windows overlap to make the screenshot smaller). I did not do any edititing of screenshots, just grabbed both windows in one go.
@paulvdh You found a footprint for the phoenix connector. There is no guarantee that the RND connector is compatible with it. (Even slightly different order numbers at phoenix are not compatible with the footprints as there are versions that require different drill sizes, this is why the compatible order numbers are listed in the footprint description.)
@ygoe if RND can not give you a dimensioned drawing of their own product, then I highly suggest not to buy their products. It simply can not be that manufacturers do not provide even the most basic documentation. The phoenix connectors that are in the lib are available at mouser which sells to private customers.
Edit: found a datasheet on distrelect They give a lead size of 0.8mm squared nominal -> diagonal is ~1.14mm -> lets assume a tolerance of 0.05mm which means we are at 1.19mm before adding space for solder and drill tolerance. I would suggest hole sizes of at least 1.4mm. The phoenix footprints use 1.2mm which means they are not usable for the RND connector. (I did not check any other dimensions but i suspect there might be differences here as well.)
I’ve found that data sheet as well, but it lacks the important part of how far the pins are inset to the outer rectangle. That defines where exactly the plastic block will be located and how much space I need to keep clear on the top side. But then, RND also suggest 1.2 mm hole diameter. When ordering I wasn’t too aware of these issues. I was rather lucky to find a connector that I could use, and quickly threw it into a pending order.
Parts should arrive here tomorrow (delivery service decided to make some trouble). I can try and measure it directly then.
Ah, RND is a brand name. I overlooked that. The error is mine.
I’ve also bought similar connectors (the 5mm variant) from Aliexpress. Different batches from those connectors were clearly clones from different manufacturers, but I had no trouble with fitting.
Also, I never trust the external libraries. I do use them, but always verify used footprints myself.
I also agree with learning to use the Footprint Editor to make your own footprints. Once you have the measurements of your connector it’s pretty easy. It just works as epxected when you have some experience with KiCad. So it’s just drawing a few pads and graphics lines.
And even that can sometimes be short circuited by using one of the Footprint wizards.
Parts arrived today. The dimensions seem to fit well. Comparing the footprint measurements with real measurements is pretty identical, the plastic block is a tiny bit smaller. The lead position should match and its thickness is around 0.82 mm (squared), with a diameter of just below 1.10 mm. So I expect things to work like this.
Yes! I will confess that I am too lazy to thoroughly investigate all of the options for this connector family, from this particular vendor . . . . . but I have some experience with other connectors of a similar style. The cable side may have wires parallel to the board surface, or perpendicular to the board. They may mate flush to the board, or hang over the board edge. These factors need to be considered before starting to place components.
Yes, making custom footprints for each variation of the mating cable side will lead to a proliferation of footprints. The alternative is to ignore the mating cable-side section, and remember to make allowances for it as we lay out the board. Some of us have better memories than others when it comes to remembering these details, and some of us have effective Design Review Committees to help us remember. Others spend a lot of time sorting through very similar footprints to find the correct one for a particular choice of components.
This situation with pluggable terminal blocks is not unique within the industry. Consider the lowly and venerable TO-220 transistor package. Three simple, through-hole, pads - correct? But sometimes they are mounted vertical (perpendicular to the board), and sometimes horizontal (parallel to the board). And, horizontal with tab down, or horizontal with tab up. With, or without, a thermal pad under the tab. Collinear pad holes, or offset-staggered pad holes. And we haven’t touched on the question of SDG versus GDS pinout. That “simple” footprint has become an entire clan of footprints!
And that’s why Forum members regularly advise new users to learn how to draft footprints and symbols. Even if a PCB layout program comes with a library of a zillion footprints, it won’t take long to find a part which requires a footprint or symbol that is not in the library.
