Texas Instruments BQ2407x

[jeanthom]

Hello,

Here's a symbol for Texas Instrument's BQ24072 and BQ24073 battery charger ICs.

Datasheet

---

All contributions to the kicad library must follow the KiCad library convention

Thanks for creating a pull request to contribute to the KiCad libraries! To speed up integration of your PR, please check the following items:

• Provide a URL to a datasheet for the symbol(s) you are contributing
• An example screenshot image is very helpful
• Ensure that the associated footprints match the official footprint library
  • A new fitting footprint must be submitted if the library does not yet contain one.
• If there are matching footprint PRs, provide link(s) as appropriate
• Check the output of the Travis automated check scripts - fix any errors as required
• Give a reason behind any intentional library convention rule violation.

[myfreescalewebpage]

Hi @jeanthom , thanks for contributing,

A few comments I have during my review:

• According to packaging information, the device should be named BQ24072RGT and BQ24073RGT to not get troubles if the manufacturer add packages options in the future
• Footprint should be VQFN, not QFN, probably something like VQFN-16-1EP_3x3mm_P0.5mm_EP1.6x1.6mm is great, it does not exist, you should propose it in the footprint repo
• Footprint filter have no leading star
• Pins length should be 100mil only (symbol < 100pins)
• BAT pins should be stacked
• PGOOD and CHG pin can't be on the top of the symbol, on the right is good
• BAT, ILIM, ISET, TMR and TS should be Passive to avoid ERC errors
• You are currently violating S3.1 that can be easily corrected by centering the symbol

Cheers,
Joel

[jeanthom]

I updated the symbol, to address most of your comments:

I don't think I will be able to properly center my component as its center is not on a 100mil grid.

Regarding BAT pin stacking, I read on KiCad's website that you can't do pin stacking with pin types other that Power input/Power output/Output. The battery pin is both a power input and output (this chip charges the battery, but also draws current from the battery). Should I keep the two BAT pins separate ?

[myfreescalewebpage]

Rules for pin stacking are at http://kicad-pcb.org/libraries/klc/S4.3/ and do not specify that only Power pins are concerned. However, there is a special attention to Power pins due to ERC checks to not get errors.

Exemple of similar device with correct pin stacking: LTC4156.

Joel

[jeanthom]

Thank's for the explanation. I set the BAT pins to Passive and stacked them up:

[myfreescalewebpage]

Hi @jeanthom thanks for the fixes.

Several point not addresses yet. Additionally:

• I do not agree with the footprint, the expected one do not exist, you should submit it (using the scripting method for this one)
• The footprint filter should not contains the number of pins, and no "-". It will be * VQFN*1EP*3x3mm*P0.5mm* for this part.

Cheers,
Joel

[jeanthom]

Hi,

I fixed the footprint filter, but I don't understand why VQFN-16-1EP_3x3mm_P0.5mm_EP1.68x1.68mm is not the right footprint. It seems to fit perfectly the datasheet's drawings:

[myfreescalewebpage]

@jeanthom the EP size is not the same. 1.6mm <> 1.68mm, even if it is a small difference, a new footpritn should be created.

[jeanthom]

Damn... Thanks for your perceptiveness, I will submit a footprint ASAP

[myfreescalewebpage]

@jeanthom any news here about the footprint ? If you have created a footprint pull request, can you give the link here ? Thanks, Joel

[myfreescalewebpage]

@jeanthom ping :)

[evanshultz]

Should IN be on top and PGOOD and CHG not? My understanding of KLC (http://kicad-pcb.org/libraries/klc/) is that power pins are on top so perhaps the request above was asking to put the open drain pins at the top of a side, and not the top of the symbol?

[myfreescalewebpage]

@evanshultz my request was to get open drain type on the right side yes, usually they are at the bottom of the right side in the library.

[jeanthom]

Hi! Sorry for the delay, I was busy for the last couple of weeks.

I haven't got time yet to create the footprint nor rework the symbol, I hope to get both done by the end of April.

[myfreescalewebpage]

No worries @jeanthom your pull request remains open, take your time to do it :) Thanks for your message!

[myfreescalewebpage]

Footprint has been proposed by another contributor: KiCad/kicad-footprints#1605
Just need to update the footprint here.
Joel

[jeanthom]

Thanks for the information, I think I did the needed changes to use this footprint. Let's hope that the CI goes right :)

[myfreescalewebpage]

Thanks, looks great ! Just notice one of my previous comment is not correctly written:

• PGOOD and CHG pin CAN'T be on the top of the symbol, on the right is good

Can you fix it please ?
Cheers,
Joel

[myfreescalewebpage]

@jeanthom any news here ? Please also solve the branch conflict to continue.

[myfreescalewebpage]

@jeanthom ping !

[myfreescalewebpage]

No news of the original author, indicate the PR is abandoned.

[RICCIARDI-Adrien]

Hi,
This pull request adds BQ24072 and BQ24073, but they are now in library (see commit cb31404). This pull request may be closed.