topic Re: MLF32 adapter in EAGLE Forum

MLF32 adapter

Anonymous — Wed, 20 Nov 2019 12:15:51 GMT

I am trying to create a very small adapter board using eagle 7.7. I am not a novice at using eagle.

I have a board with an SOIC28 mcu that is being replaced with an MLF32.

The small adapter board is the size of the SOIC28.
The MLF32 is mounted on the board. The adapter board will have castellated holes and mount in place of the SOIC28 mcu.

I have created the board, however due to limited space, there simply is not enough room to place any more vias for the remaining pins. I only need to run 4 more tracks.

This is a 4 layer board. Currently i am using top and bottom layers.

I would like some advice on what to do with the remaining pins since there is no room to place more vias for layers 2 & 15. I have read many tutorials however I can't find the answer. I require more vias to be placed that will not interfere with other layers.

Any advice would be greatly appreciated.

Thank you in advance.

Re: MLF32 adapter

rachaelATWH4 — Wed, 20 Nov 2019 15:42:35 GMT

@Anonymous wrote:

The small adapter board is the size of the SOIC28.
The MLF32 is mounted on the board. The adapter board will have castellated holes and mount in place of the SOIC28 mcu.

Ok so the first thing that stands out to me is that you have the SOIC28 pads on there. You don't need these, you just need the PTH for the castellated pads. So if you get rid of these and possibly edge the castellations out slightly (check to ensure you have enough space for a good solder joint if you do) you'll regain yourself a lot of space.

Then if you have enough space I would consider whether rotating the MLF32 anticlockwise by 45 degrees will also help as it'll get more clearance around its pins and possible give you more space for vias. Use the unused inner layers for your power/ground connections, thermal/ground vias in the centre pad (assuming your vias are small enough so they don't wick the paste or have them filled) to help get that connected up without additional vias around the outside for ground.

These are just a few things off the top of my head from a quick look over it. It looks to me like what you are trying to achieve should be doable with a little tweaking.

Best Regards,

Rachael

Re: MLF32 adapter

Anonymous — Thu, 21 Nov 2019 00:02:41 GMT

Thank you Rachael for your advice.

I did have the MLF32 turned 45 degrees but it didn't seem to help. I will try it again once I remove the SOIC28 pads.

Great advice, thanks again.

I heard horror stories from others who placed vias in the thermal pad.

Too much paste on the thermal pad (caused by the vias) can raise the MLF device and can prevent the other pins from making good connections. I don't know for sure because I never made a board with an MLF device before, however it does make sense.

So the correct way to do casellations is to just place a via in the outline of the device?

When the board manufacturer cuts the board, they leave the vias exposed?

As always any adviced is greatly appreciated.

Re: MLF32 adapter

rachaelATWH4 — Thu, 21 Nov 2019 18:54:44 GMT

@Anonymous wrote:

I heard horror stories from others who placed vias in the thermal pad.
Too much paste on the thermal pad (caused by the vias) can raise the MLF device and can prevent the other pins from making good connections. I don't know for sure because I never made a board with an MLF device before, however it does make sense.

So the issues you can have with thermal pad of the MLF are:

1) Too much paste on the centre pad. This is not caused by the vias it is caused by the paste mask being too open in that area. You probably want to put a 2x2 grid of paste with a coverage of say 50-70% of the pad. The device datasheet will give recommendations here.

2) Too little paste. This is caused by thermal vias with too large drill size causing the paste to be wicked away from the pad. Speak to your PCB vendor and see what they recommend is the smallest drill which doesn't cause the price to be hiked up too much. I try to keep vias in thermal pads to 12mil to avoid wicking. You can also have the vias filled too to try to avoid this. Speak to your PCB vendor to work out what is most cost effective.

@Anonymous wrote:

So the correct way to do casellations is to just place a via in the outline of the device?
When the board manufacturer cuts the board, they leave the vias exposed?
As always any adviced is greatly appreciated.

I wouldn't recommend using vias. Create an alternative footprint using TH pads which will ensure that the annular ring isn't covered with solder mask and it'll allow you to map symbol pins to it properly so you're less likely to insert accidental connectivity errors. The board edge will then plough straight through the centre of all these pads. Tell your PCB vendor what you are intending here.

@Anonymous wrote:

When the board manufacturer cuts the board, they leave the vias exposed?.

Talk to the manufacturer so they know what your intention is and they should get it right.

Best Regards,

Rachael

Re: MLF32 adapter

Anonymous — Tue, 26 Nov 2019 12:38:00 GMT

Well after moving components around and starting over from scratch numerous times, I finally got the board down to two layers only. I didn't need the third and fourth layers.

Thank you for responding to my post.

Re: MLF32 adapter

rachaelATWH4 — Tue, 26 Nov 2019 14:08:53 GMT

Excellent, that's good to hear, glad it all worked out 🙂