I’m building a PCB that contains a large relay. Its dimensions are 38x35mm and the pins are spaced at two different pitches-- 6 pins at 7.8mm and the coil pins at 5.5mm.
Since I could not find the TE Connectivity 15722B200-R2918 relay in the Footprints list, I tried to design my own. However, the template I used must have been for SMD device as there are no thru holes.
The second issue is that there are no net connections.
This is what I get as a result, relay is missing and only SMD pads on board:
How do I make holes and connect the nets so there are electrical connections?
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.
If you scroll down the page, you will see there is a version available to directly solder into a PCB. Is that available? If so, there is a PCB template shown.
I’ll comment in the next post on creating a footprint.
When you create a footprint, you have to specify whether it’s for a surface-mount or through-hole device; I suspect you missed this step. And it looks like your wiring is all on the bottom layer, while the SMT pads are all on the top, so there’s no way to connect these.
In the footprint editor, take a look at your footprint’s properties (type “E”) and change the component type:
Once the component type is fixed you can modify the footprint as needed. You should make sure the pad names/numbers are correct (see Footprints - Library Conventions | KiCad EDA for information on this - I believe there are special rules for relays).
From the datasheet it looks like this relay is normally socketed, it’s possible that the Relay_Socket_4PDT_Omron_PY14-02 footprint will be suitable for the matching socket, but you’ll have to do your own homework for this.
This is how I would create a footprint according to the PCB layout at the bottom of your data sheet.
Find a relay (any relay) in the Kicad library. RMB, then select “Save as”. Give the relay a new name, highlight your personal library, press Enter.
Open this relay in your personal library and move the relay to one side of the workspace. This is your “cheat sheet” to remind you of all the lines and layers required.
Set up three new grids. X = 11.04 Y = 5.58, X = 11.04 Y = 13.71, X = 11.04 Y = 21.33. These are the pad spacings on the data sheet. To do this click on the arrow in the grid display at the top of the worksheet (green arrow). At the bottom “Edit Grids”. At the bottom of the grid list in the new window click the + sign. Untick “Linked” fill in X & Y and OK.
Select new grid X=11.04 Y= 5.58.
Place “Add Pad” open Properties of pad. Make THT, give it number 1, select size and shape and hole diameter. (I used X=5 Y=4 round rectangle hole = 2mm)
Place first 6 pads using this grid. Pads will automatically land in their correct position with their correct numbers.
NOTE: the data sheet shows the bottom view but you are creating a new footprint with the top view, so numbers are reversed)
Change grid to X=11.04 Y= 13.71. Place pads 7,8 & 9.
Change grid to X=11.04 Y= 21.33. Place last two pads and rename.
Change grid to suitable small grid to draw your three outlines according to the “Cheat sheet” relay (I’ve only drawn the F.Fab). Start with F.Fab as the overall size of the relay cover. ( I used 36mm X 39mm)
When you have finished all the drawing, delete the “Cheat sheet” relay and save the new relay.
Job done.
At the time of my search on Mouser’s site, this was the only relay I found that had the needed specs. I also wanted a plug in for easy replacement should this one fail at some point.
I’m going to take tomorrow to digest your followup post and do some mockups of the relay.
I’ve sent requests to Mouser and TE Connectivity for the socket part number and also if they have footprint files. A lot of their product does. But I’m taking this as an opportunity to learn how to make my own for situations where none are published.
Good to hear.
Making footprints and symbols are really easy after just a little practice and, usually, much quicker than surfing the net to find something suitable.
It is often even easier to modify existing kicad footprints. Use “Save as” or Copy/paste the Kicad library part.
Most of the basic stuff is covered in the “Beginners Guide” but if you ever have problems creating footprints and symbols, ask on this forum. You’re bound to get at least 10 different, but correct, solutions.
