Add VSON-10 for ROHM BD8314NUV

[asukiaaa]

Datasheet: http://rohmfs.rohm.com/en/techdata_basic/ic/package/vson010v3030_1-e.pdf

Related PRs:
KiCad/kicad-symbols#934
KiCad/kicad-packages3D#401

• Provide a URL to a datasheet for the footprint(s) you are contributing
• An example screenshot image is very helpful
• If there are matching symbol or 3D model pull requests, provide link(s) as appropriate
• Check the output of the Travis automated check scripts - fix any errors as required

[Misca1234]

Is this not supposed to have thermal vias, according to page 6 (and therefore get the file name ending '_ThermalVias') ?

[DanSGiesbrecht]

I found a few concerns with this footprint (shown below). Also, I agree with @Misca1234 - it may be valuable to add a footprint with thermal vias.

[DanSGiesbrecht]

The name should be VSON-10-1EP_3x3mm_P0.5mm_EP1x2.1mm - EP dimensions should be listed in X,Y order. Also, consider adding the component height of 1mm.

[DanSGiesbrecht]

Silkscreen lines are overlapping copper pads, which is not permitted.

[DanSGiesbrecht]

It is recommended (in the KLC) to have a bevel of either 1mm or 25% of the shortest side of the part (whichever is less) on the fab layer to indicate pin 1, which is currently missing.

[DanSGiesbrecht]

The courtyard should provide mechanical and electrical clearance. Currently, the courtyard is not accounting for the copper pads on the sides of the part. The apparent clearance of 0.25mm from the body of the component should be used for the copper pads as well.

[DanSGiesbrecht]

The EP dimensions are incorrect, and in the wrong order. They should be: VSON-10-1EP_3x3mm_P0.5mm_EP1x2.1mm. This will require a change to the 3D model name in your other PR. Also, as above, consider adding the component height of 1mm.

[DanSGiesbrecht]

I would recommend replacing the packaging datasheet (currently listed) with the full datasheet (found here). The packaging datasheet doesn't have any information about the actual package size, only the land pattern.

[asukiaaa]

Thank you for a lot of comments.
I updated according to your comments except for datasheet url.

I assign BT8314 datasheet to symbol but assign package datasheet to this footprint because I think that VSON package does not need to know BD8314 detail.
How do you think?

[DanSGiesbrecht]

I agree that the BT8314 datasheet has more information than strictly required, but my understanding is that the datasheet linked in the footprint should contain enough information to create that footprint, which includes dimensions for the fabrication layer. The package datasheet doesn't contain any dimensional information for the package itself (width, length, height). It only contains information for the land pattern (footprint).

The BT8314 datasheet contains the required information about package dimensions:

(source: http://rohmfs.rohm.com/en/products/databook/datasheet/ic/power/switching_regulator/bd8314nuv-e.pdf , page 20)

I think that the BT8314 datasheet should be included in the symbol and footprint. It may be valuable to link to both datasheets. Other maintainers may have feedback on this.

[poeschlr]

This part could easily be script generated by adding the size definition to this script: https://github.com/pointhi/kicad-footprint-generator/tree/master/scripts/Packages/Package_DFN_QFN

[Misca1234]

@asukiaaa
Do you want me to do a script based fp (if you don't know how to do it, you will see how easy it is) ?

[evanshultz]

First, as I've noted elsewhere, the footprint name is wrong. The EP size is 1.2x2mm.

Next, we will use a generic package drawing to reference in the datasheet if possible, and if not then a datasheet with the package drawing. In this case, I think we can use the datasheet. A quick Google search for "VSON010V3030" turns up https://d1d2qsbl8m0m72.cloudfront.net/en/techdata_basic/ic/package/vson010v3030_1-e.pdf, but that doesn't have the package drawing. (I believe this is what Dan mentioned above and called the "package datasheet".) And we would use an official URL from ROHM anyway.

Because symbols are specific to a particular part, the datasheet should always be there.

That all being said, rather than use the footprint supplied from a vendor we can generate a footprint according to IPC rules as Rene wrote above if we just have an adequately-dimensioned package drawing. In this case, I've made the footprints and attached them (with .txt extension added) using the YAML entry given below at kicad-footprint-generator\scripts\Packages\Package_DFN_QFN\size_definitions\dfn.yaml. While I took a look and they appear correct you should verify them as well. While making footprints manually is still OK, the IPC-compliant generator is best and the future direction of the KiCad footprint library.

VSON-10_3x3mm_P0.5mm_EP1.2x2mm:
  device_type: 'VSON'
  #manufacturer: 'man'
  #part_number: 'mpn'
  size_source: 'http://rohmfs.rohm.com/en/products/databook/datasheet/ic/power/switching_regulator/bd8314nuv-e.pdf (Page 20)'
  ipc_class: 'qfn' # 'qfn_pull_back'
  #ipc_density: 'least' #overwrite global value for this device.
  # custom_name_format:
  body_size_x:
    nominal: 3
    tolerance: 0.1
  body_size_y:
    nominal: 3
    tolerance: 0.1
  lead_width_min: 0.21
  lead_width_max: 0.3
  lead_len_min: 0.3
  lead_len_max: 0.5

  # heel_reduction: 0.05 #for relatively large EP pads (increase clearance)

  EP_size_x_min: 1.1
  EP_size_x: 1.2
  EP_size_x_max: 1.3
  EP_size_y_min: 1.9
  EP_size_y: 2.0
  EP_size_y_max: 2.2
  # EP_paste_coverage: 0.65
  EP_num_paste_pads: [2, 2]
  #heel_reduction: 0.05 #for relatively large EP pads (increase clearance)

  thermal_vias:
    count: [1, 2]
    drill: 0.3
    # min_annular_ring: 0.15
    paste_via_clearance: 0.1
    EP_num_paste_pads: [2, 2]
    #paste_between_vias: 1
    #paste_rings_outside: 1
    EP_paste_coverage: 0.75
    #grid: [1, 1]
    # bottom_pad_size:
    paste_avoid_via: False

  pitch: 0.5
  num_pins_x: 0
  num_pins_y: 5
  #chamfer_edge_pins: 0.25
  #pin_count_grid:
  #pad_length_addition: 0.5
  #suffix: '_Pad{pad_x:.2f}x{pad_y:.2f}mm_HandSolder'
  #include_suffix_in_3dpath: 'False'

Sorry @Misca1234 , I started this post a few hours ago and was just able to wrap it up now.

VSON-10-1EP_3x3mm_P0.5mm_EP1.2x2mm.kicad_mod.txt

VSON-10-1EP_3x3mm_P0.5mm_EP1.2x2mm_ThermalVias.kicad_mod.txt

[Misca1234]

@evanshultz
No problem

@asukiaaa
Do you understand how the script generation works and what you need to do?

[evanshultz]

If you do use the footprints I posted above, here is an image and dimensioned drawing:

[evanshultz]

I pushed a script update to add this footprint at pointhi/kicad-footprint-generator#182.

That shouldn't preclude you from playing with the scripts yourself and trying it out if you like. :)

[asukiaaa]

Thanks for the comments.

I understand them.

• There are scripts to create footprint.
• Datasheet of BD8314FNG is needed to know package size.

It take me a long time to run script but I succeeded for FQN.

git clone https://github.com/pointhi/kicad-footprint-generator.git
cd kicad-footprint-generator
./manage.sh update_dev_packages
./manage.sh tests
cd scripts/Packages/Package_DFN_QFN
./qfn.py qfn.yml
ls Package_DFN_QFN.pretty/

By the way, this PR is not needed now because other PR including this was created?
#958

[evanshultz]

I only created a PR for the script for this footprint. The footprint itself hasn't been added so you can replace the footprint you committed with the one I attached above it if you wish. Or if you prefer to close this PR I can submit the scripted footprint in a new one. Either way is OK with me.

I'm just happy you were able to figure out how to run the script and generate footprints. I think you will find this is the most powerful way to generate new footprints of this type as you need them. If you have questions please ask!

[Misca1234]

@asukiaaa
You need to do the following

1. Use the same data in evanshultz push Add THAT Corp & ROHM QFNs pointhi/kicad-footprint-generator#182

2. Create a foot print as you have just learned with this data (unchanged)

3. Replace the content in this push with the .kicad_mod file that you produced with the script

4. If needed, rename the file of the 3D model in push
   Add VSON-10-1EP_3x3mm kicad-packages3D#401
   to match the foot print file

[asukiaaa]

Thanks for the comment but I close this PR because other PR was created and merged.
I'm sad.

[evanshultz]

@asukiaaa
Sorry to sadden you! I did not mean any offense.

I'm happy that you were able to get the scripting sorted out and I should have been more careful when I pushed the footprints to exclude this one. I was going too fast and pushed all the QFNs I'd generated into one branch.

I'm thankful that you took initiative to add symbols and footprints to KiCad. Having people like yourself add parts they need into our library is important to making a useful library. I hope to see more contributions from you in the future that will grow and improve KiCad's official library for all users. :)

[asukiaaa]

Thank you, I'm glad to know that.