I have a footprint that I downloaded from DigiKey (255-1939-ND) and is the same footprint available in librarian.
https://www.digikey.com/en/products/detail/panasonic-electric-works/CP1-12V/647155?s=N4IgTCBcDa4KxwLQEYCcBmViByAREAugL5A
This footprint is for a CP1-12V solenoid and requires three slots and two standard holes. When I attempt to route connections DRC error occurs. The problem is in the through hole slots required for assembly. I have attempted several times to use multiple drills and edge cut but all results fail.
A single drill large enough is a very large diameter and will not work as it will leave too much room needed for solder.
This appears to maybe be a two drill operation with a small milling movement required to remove whats left in between the two drill holes then add solder mask to a rounded rectangle and enable through hole plating?
This link points to a png of the footprint CP1-12V footprint Pins 2, 3, and 4 are what need to be resolved.
How can this be accomplished?
This should work. Could you show your PCB and your DRC error?
Here is a png of the DRC failure DRC Failure
Here is a png of a section of the PCB with the CP1-12V PCB Section
could you please attach them in the forum so I don’t have to connect to your synology NAS?
ins 2, 3, and 4 are what need to be resolved. How can this be accomplished?
You will have to modify and correct the FP yourself. It seems the pad was originally drawn as a pad plus two additional NPTH holes inside this pad. You should delete this construction and replace with a simple PTH pad. Set the pad shape to oval and hole shape also to oval.
This the relevant chapter in the documentation: PCB Editor | 8.0 | English | Documentation | KiCad
You may also look into existing footprints from the standard kicad library. For example USB3_A_Plug_Wuerth_692112030100_Horizontal (library connector_USB) also offers throughole slots.
And regarding your attaching something: please include pictures directly into your message, not as link which might vanish over time. To attach multiple images you will need a higher user trust level. Read and follow this FAQ article: New Member Information to prmote yourself to basic user level.
@mf_ibfeew - I will take a look and see how to make that change - thanks
@mf_ibfeew - After a quick overview I think I see how to address this. When completed I will add a link to the updated footprint. As I do this is there a convention I should follow in the naming and is there a place to put this for other KiCAD users who may use this footprint?
Changes made to Footprint. I was able to complete PCB Routing and successfully eliminated DRC errors. For anyone who finds this thread I include the following information to the pads of the CP1-12V Footprint. The X and Y position data is relative to the position of the model I have. You need to open each existing pad to get that information which will change if you moved the orignial Footprint model.
CP1-12V
PAD2: POSX= -2.34958 mm POSY= 4.4958 mm
PAD3: POSX= 2.9972 mm POSY= 9.906 mm
PAD4: POSX= 8.3439 mm POSY= 4.4958 mm
PAD shape: Rounded Rectangle
Corner Size: 50 %
Corner Radius: 0.6985 mm
Pad Size: X:2.1546 mm Y:1.397 mm
Angle: 90
Hole Shape: Oval
Hole Size: X:2 mm Y: 0.9 mm
Copper Layers: All copper layers
F.Mask
B.Mask
Thanks to @mf_ibfeew for pointing me in the right direction.
The moral of this tale, seems to me, is to just use the footprint editor from the beginning - measure and place three slots and two pads, draw a courtyard and job done. So many people spend hours searching for a footprint (or even worse, a symbol) to import from some slightly dodgy website when they could use the time learning to draw your own symbols and footprints. I do understand there is some reluctance to delve into what seems like a dark art but if the component isn’t a standard one, a few minutes with the symbol and footprint editors is time better spent than a fruitless hunt - gradually you will get faster at drawing suitable representations. I know, I’ve done the same myself but drawing your own is a very useful skill.
6 Likes
@John_Pateman - I hear that and I have also spent time searching until I started using tools available to make or modify. I have used many SCH-PCB applications and there are varying degrees of difficulty in using such tools. I will say that I find using KiCADs Footprint editor one of the best I have ever used.
When @mf_ibfeew mentioned modifying and included a link to documentation the process literally took me less than a half hour.
I actually took more time to “clean up” and arrange elements as I desired. It was really simple and straightforward duplicating the original model, modifying then saving. Both models are available and are next to each other in the Library simply by appending “_KiCAD” to the Footprint name.
This update included changing the SCH model to include MPN, Data sheet link and the updated Footprint.
This all took less than a half hour and I have what I need. So yes I agree especially with KiCAD. This is my first time seriously using KiCAD and I have made the decision to end using several other applications in favor of KiCAD. Use, learn, and get it done
3 Likes