Then I looked at the footprints that are in KiCAD.
I found: Housings_DFN_QFN:DFN-14-1EP_3x4mm_Pitch0.5mm
This is probably close, but not close enough. The casing of the real part is 3x3mm instead of the 3x4mm in the library, but that is probably not a problem as long as the pads are in the right place. But they are not, because the pitch is wrong.
Pfff. Does anyone have a suitable footprint for a 14-DFN 3x3mm pitch 0.4mm that could be donated to the lib’s, by any chance?
I really, really like standardisation but the manufactureres of SMD parts seem to use different naming conventions and invent packages as we speak.
I need a break. I am about to drop the MAX9814 altogether…
No, Autodesk Inventor, but I got free access via a university. If that wasn’t the case I’d be using FreeCAD. But unless there is pressure one usually sticks to the tools one knows and has become efficient in
PS:
I just followed the links in the DS for the land pattern and package drawing… no landpattern to find, I get the package 2 times.
Creating it with the FP editor isn’t a big deal, grab the 3x4 DFN package for the VAL/REF fields, remove all pads sans #1 and use the array function to create the new pattern.
Adjust the silkscreen, fab and crtyard a little and you’re done.
Takes 5 minutes tops if you got experience… 10 minutes if you’re rusty and 15 if your new to this
…oh, and 5 min more for searching the correct land pattern
The footprint is probably doable, yes, that is probably the easy part. The 3D image is what was worrying me. I guess I will have to get myself into FreeCAD, sigh.
And then I need to find out how to contribute a footprint to the KiCAD repo’s.
Doable, I’m sure.
m
In the mean time… for someone firmly into standards, it is disappointing to see the mess SMD seems to be in. And it seems to get a bigger mess by the day. Sad.
Please don’t do that! The MAX9814 looks like an excellent electrical choice for a project that’s on my desk right now, but was passed over due to the tiny packaging. I just got some hints of what features marketing wants to put into this project’s long-term development, and it’ll be necessary to reduce component sizes so I may be revisiting the MAX9814 in the future.
The proliferation of packages is painful in it’s own right. And none of the SMD packages seem to disappear, or at least become so uncommon that they can be forgotten. (E.g., TO-3, TO-5 and TO-39 are still “on the books” of manufacturers and standards organizations but are so rarely encountered that few people will ever miss them if they don’t show up in an EDA library.)
To make matters worse, manufacturers fabricate cutesy names for THEIR versions of packages that are used by other manufacturers. That’s akin to the different naming conventions problem you mentioned.
It has some neat functionality, I agree, @dchisholm .
The component is ready for use, except for the footprint.
I will give the footprint a swing tomorrow, but the 3D might take a while.
In the mean time, we could perhaps discuss in which library we want the MAX9814 to appear.
It is a linear device, intended for audio use -> audio.lib is the most logical place, I think.
But perhaps there are people that would prefer maxim.lib?
m
Allright, the footprint is done, except the 3D part.
I will check everything tomorrow and if I am satisfied I will push to the repo’s and do the pull request.
The 3D remains to be done.
m
@mifi I’ll script a 3d model for you when it has been approved (I’m the one who added all the other QFN and DFN) unless you want to try it out yourself
I am battling with the Not Connected pins.
According to the KLC, the must be set to invisible (rule 4.7.iii).
However, the datasheet explicitly mentions they should be connected to GND, and hence they must be visible:
I am probably not the first one to run into this conflict in KiCAD.
I did notice a small discussion last Januari (NC (no connect) pins?), but it does not deal with the fact that an NC is to be connected and invisible at the same time.
And this thread (NC pins layout, please help) touches it, but not exhaustively.
What do I do about this?
Setting the NC pins to invisible and leave them unconnected in the schematic would violate the datasheet.
Renaming them GND and stacking them with pin 7 would be a solution, but that makes the relation with the datasheet unclear, because the datasheet names them NC.
Setting the NC pins to invisible and have the PCB designer create extra GND connections in pcbnew to the NC pins and the Epad, as recommended in the datasheet. I believe this is the current status quo. I do not like the idea that not all electrical connections are in eeschema, but it is like it is, I guess.
No problem, you should still add a reference to the 3d model, it will do nothing if there is no model but will ease it quite a bit when somebody needs to add the model
Yes, I will do that when the 3D model exists. the KLC does not allow me to do that any sooner, does it. I believe I had the scripts fail on me when I did this, but I am not sure.
No according to KlC you should always have a reference to the 3d model, I’ll check the tracis script and see if I can help you out
I’ll write them on git
but the manufactureres of SMD parts seem to use different naming conventions and invent packages as we speak.
