I am trying to put a PCB transformer into a design. I’ve found some suitable symbols, e.g. Transformer_SP_2S and TRANSF8, and I’ve found a nice footprint that matches the EI54 brick I intend to use (Trafo_CHK-EI54-12VA-*). However, the pin numbers do not match between symbol and footprint.
Given that these are all library symbols/footprints, I assume I am not meant to modify them lest my changes be lost… How do I make these link up between schematic and PCBs? Is there a way in cvpcb to map/transf pin numbers between symbol and footprint? Unless I’m missing something basic here, the default symbol/footprint libraries for transformers seem broken or incompatible with each other.
Do I need to make a private copy of the footprint with my own renumbering?
I have never asked myself such question. I just copy all I plan to use to my libraries and modify if needed and use only symbols/footprints from my libraries. That way I believe I am 100% protected against any changes in KiCad libraries.
I agree with Piotr. Also understand that it if you figure out how to modify a footprint or symbol in the standard library, your modifications are likely to be lost when you update KiCad. Make your own personal KiCad libraries, modify and put symbols and footprints in those libraries, and use them. I have posted my own symbol libraries in another post recently but I doubt anyone else is using them.
A word of caution. Transformers are one of the most likely devices to be designed in upside down.
When you’ve finished your board, print out the Gerbers or layers at 1:1 and physically sit a transformer on the paper to verify the connections are correct. Many folks (including myself) have learned this the hard way. Especially with custom transformers.
Seriously though; I think the issue may be nonstandard pin numbering? 2-row connector pin numbers for example are not numbered like a DIP IC. I think that is because they make and sell many different connector sizes/pin counts.
Why use a PCB transformer at all?
Mains voltage entry usually needs a connector or pulling strain relief, a switch and a fuse before the transformer. The fuse could be on the PCB but the rest usually is not.
For hobby projects it’s much more convenient to tug the transformer away in some corner of the cabinet, and then use a low voltage cord to connect to your PCB. This makes it much easier to do fault finding or repair on your PCB because there are no high voltages on it.
Quite often you can also power it from a DC bench power supply through the AC input during “maintenance”, and the PCB is also a lot smaller and lighter.
I do not know the skill level of the person who made the original post, but I will sometimes take something like a PQ-2625 bobbin and wind a transformer for use in my own high frequency power converter. This converter may or may not be isolated, and may or may not use AC mains voltage. Anyway a high frequency transformer such of this will generally need to be located on the pcb so as to minimize layout inductance. In this situation mounting the transformer off the board does not seem to be helpful.
Yes, and place your symbol in your personal schematic library and your footprint in your personal footprint library.
When you have made both your symbol and footprint, go into your symbol properties and place the link to your footprint in the “footprint value”. All you have to do is click on the value box which will allow you to search through all footprint libraries, including your new personal footprint library.
Not really.
After you have saved the transformer footprint into your personal library (use “save as”) just edit (rename/number) the pads to match your transformer and symbol.
If you have not yet made your personal libraries there are comprehensive instructions in the FAQ at the top of this forum page.
I have plenty of personal libraries for actually custom/unusual parts, and left over from KiCad 4 when there was approximately nothing available by default.
Creating my own personal symbols for a DIN standard transformer is somewhat grating though - in the same way that I do not need to create my own TO220, SOIC, DIP, 0805, etc, footprints… I should not have to hack around to get alignment with a widely-supported DIN standard footprint, particularly when both footprint and symbol are already in the standard libraries.
When I started to be interested in KiCad (4.0.7) I noticed that here I have separate 0603 footprint for resistor and separate for capacitor. Before (in Protel) I used one for both and newer even got an idea to have two different. The resistor 0603 I liked specially as there were 1mm distance between pads that I noticed - using 0.2/0.2mm (track/clearance) I can go with two tracks under resistors what was newer possible for me before. Capacitor 0603 had bigger pads and smaller gap. I found datasheets with exactly such footprints but don’t remember now what producers those were. I asked my contract manufacturer and they didn’t accepted that resistor footprint as resistors from different sources have a little bigger contact areas and smaller distance between pads in their suggested footprints.
So thinking - why to define footprint if it is already done can be risky.
In V5 that footprints were changed.
I have also other reason to copy footprints to my libraries. Before first time using KiCad I spend some time thinking how footprints should be done to easy generate documentation we need, and KiCad footprints do not fit my requirements. I’m sure that for V4, and almost sure for V5.
You do realize that different manufactures, for the same compatible part, have differing Land Pattern Data requirements??? What Land Pattern should the KiCad KLC adopt?
We outsourced our PCB design to a company with equally eye wateringly expensive CAD. They would create a library for every job from the mfg recommended footprint.
Deadly serious. I’m not asking for Every Possible Transformer, but there are some standardised footprints. For example in the EI54 series, there are 2 options for primary configuration and about 6 options for secondary configuration - from all the the manufacturers available through element14.
Yes in theory there are a bazillion combinations but in practise, all the manufacturers have converged on a very small number of common arrangements. Say you want a 1P2S in EI54, I’ve found only two variations so far from about 5 different manufacturers. Same for a 2P2S.
Guess I’ll have to chuck a library module on github one day when I’m bored.
The footprints for the “Transformer_CHK_EI…” all seem to have all pads present.
Once you’ve put such a transformer on your PCB, deleting the unwanted pads (which usually is not needed) is very easy by loading t in the footprint editor (hover over it and press [Ctrl + e].
The pins for the electrical connections of these transformers seem to be fairly standard, but the connections for mechanical mounting holes are not. For example most have plastic extrusions on the outside:
Such differences result in a lot of variations for such transformers.
For the schematic symbols, there just are no specific schematic symbols for these transformers. There are only some very generic schematic symbols for transformers, and then of course the pin numbers do not match. To “fix” this in KiCad would need different pin numbers for the variants. For example EI38 has 10 pins, EI48 has12 pins and EI54 has 14 pins.
Changing pin numbers of a transformer is also quite trivial (after it’s copied to a personal library). For me it’s just one of the many small things to check and verify in any project.
— 8<----- 8<----- 8<----- 8<----- 8<----- 8<----- 8<----- 8<----- 8<–
There does seem to be a bug in all the Footprints for the "Transformer_CHK_EI…**.
I’ve looked at a few different datasheets: https://html.duckduckgo.com/html?q=EI54+transformer, and they all specify the bottom view (Such as “view on pin side”) and then put pin 1 in the lower left corner. KiCad always uses Top view, and therefore pin 1 should be in the upper left corner. I have also verified this with a few transformers I have lying around. This is also more in line with the common counter clockwise numbering of IC’s.
