Connecting VCAP pins through GPIO pins to ease routing

[Rich Barlow]

Posted on June 15, 2017 at 18:04

Hi,

I am currently laying out a board with an STM32F413VGH (UFBGA100) microcontroller. The required pinout is very flexible and only around 50% of the IO pins are in use, which means that is should be possible to fan out the device without microvias. However, annoyingly, both of the VCAP pins are inaccessible without resorting to microvias to drop down a layer. I am wondering if it is valid to just connect each VCAP pin to a GPIO pin (i.e. VCAP_2 to PA10 and VCAP_1 to PB12) to allow them to be escaped to the periphery of the package. I've had a good look around and can't see any evidence of anyone doing this before, but I also can't see any reason why it would be a problem. The core voltage (present on the VCAP pins) will vary between 1.08V and 1.38V and all GPIOs are configured as a floating input on reset. The only potential issue I can imagine is the fact that the GPIO is being driven with an intermediate voltage (in the 'Area not determined' region of Figure 35 of the datasheet), but I expect the Schmitt trigger input to ensure that the pin doesn't enter a metastable state.

Has anyone ever connected a VCAP pin to an (unused) GPIO pin to ease routing?

Thanks,

Rich

[Tesla DeLorean]

Posted on June 15, 2017 at 20:18

Can't say I've tried it, or needed it, but it sounds like a solid approach.

[waclawek.jan]

Posted on June 15, 2017 at 20:53

I understand how far is 'tried' from 'guaranteed to work', but... unless you have incentives enough to get a binding answer from ST (which I am afraid is not the case since you ask here), the least you can do is to take a cheap Nucleo F4 board and try it there.

JW

[Rich Barlow]

Posted on June 16, 2017 at 12:26

Since it's highly unlikely that ST will ever give a definitive answer either way (I have also raised a technical support query with them) I have instead gone for the approach of reducing the pad size to 0.2mm, which allows the VCAP pins to be escaped with 0.1mm track/gap. The footprint previously had 0.28mm pads, which is what the datasheet recommends, however after reading IPC-7351 it appears that is is unnecessarily large - the nominal recommended pad size is 0.25mm with a minimum of 0.2mm. I also have also since received evidence of a design with this exact package and 0.2mm pads being successfully manufactured in volume.

Rich