Hey there ADI,
I have a question about the grounding pads for the ADMV1014 footprint. The gerbers provided with the users guide show 4 pads sort of centrally located in the part. Each of these pads appears to be roughly 55 x 55 mils and there is roughly 20 mils of spacing to the pins (see below).
There is a similar image in the datasheet (Figure 122), which suggests the same footprint design; however there are no dimensions. This footprint does NOT agree with the package dimensions in the very same datasheet (see below).
According to the datasheet, there are 16 ground pads, not 4. Also, these ground pads extend much closer to the outer edges of the package. Given the frequency range of this device, it is crucial that this footprint is correct. Should the footprint match the gerbers or the package drawing? And if the gerbers are correct, what is the reason for the difference? And can ADI provide an actual recommended land pattern with dimensions?
The Gerbers provided on the product page are of the ADMV1014 Eval Board that ADI uses and which we had success with assembling the ADMV1014. All the performance shown on the datasheet is with the ADMV1014 ICs soldered on to eval boards with the same PCB land pattern.
That is sort of what I assumed. But can someone please explain WHY the land pattern in the gerbers is different than the package dimensions? This is not normal practice and it seems odd to me that ADI would not provide a dimensioned drawing of this land pattern in the data sheet.
My concern here is that the footprint was optimized for the specific board stack up that ADI used for the evaluation board. And if my board stack up is slightly different, now what? If this were, say, 6 GHz, I probably wouldn't worry. But this is a 40 GHz part.
The 4x4 pattern on the package is determined based on packaging reliability and integrity which is not needed for the PCB and a 2x2 PCB land pattern was deemed to be better for the ground pins as it allows for a better ground contact, lessens the chance of solder voids, and creates a smoother level for the solder.
We can only provide the PCB land pattern based on our board. The PCB land pattern that is in the gerber files have been used extensively since the products release . You can use the gerber files to obtain the dimensional drawing if that is needed for your design. The gerber files facilitates quicker design as it allows the user to drag and drop the land pattern straight into the designer's PCB. If you deem it necessary that you need to redesign the PCB land pattern we recommend following IPC guidelines. (IPC documnents: IPC 7525B (Stencil Design), IPC7351 (SMT Design and Land Pattern Standards) and IPC-7093 (Design and Assembly Process)).