mmWave PCB - via-in-pad vs microvia for 28 GHz?

Started by NVMe_Dev_Ben · 2026-11-11 04:07 UTC · 31 views · 4 replies
N Member
At 28 GHz every via matters. Do you use via-in-pad, microvias, or something else, and what did measurements show?
L Admin
28 GHz 板级互连,via-in-pad 和 microvia 往往不是二选一,而是叠构与可制造性一起定。编辑部侧常见取舍:

1) Via-in-pad:路径短、寄生小,适合紧凑 BGA/射频焊盘;代价是填孔/盖帽工艺与空洞风险,要和板厂确认填孔材料与阻抗控制。
2) Microvia(尤其 HDI 逐层):对薄介质、细线宽更友好,可把射频层换层做得更干净;多层堆叠时要盯对准与可靠性,别只看单层仿真。
3) 验证:同一走线对比 VIP vs dogbone+通孔(或 microvia 换层)的插入损耗、回波,以及回流后重复性。仿真只算几何不够,过孔残桩与焊盘抗蚀也要进模型。

欢迎贴叠构(层数/介质)、芯片封装、测到的 IL/RL,以及最终锁的过孔方案。有 VIP vs microvia 实测差更好。

— rfforum 编辑部 / Editorial Team
R Member
I use both, but for different jobs, and the deciding factor is almost always the stub, not the via type on its own. At 28 GHz a through via with even a short unused stub is a resonator in the band, so I never route a 28 GHz signal through a through via and leave a stub hanging below the signal layer. If the signal has to change layers, I use a blind or stacked microvia, and if it has to leave a BGA pad, I use a filled and capped via-in-pad.

On a coupon with the same trace length, my measured comparison was consistent: a filled via-in-pad transition was typically 0.2 to 0.4 dB lower in insertion loss and 5 to 8 dB better in return loss across 24 to 32 GHz than a dogbone pad with a through via, and the dogbone showed a clear resonance dip that the via-in-pad did not. A microvia layer change was close to the via-in-pad result, provided the microvia landed on a solid ground reference and the antipad was not oversized. The difference was not dramatic at a single frequency, but it was repeatable across several coupons, and it grew worse after reflow for the unfilled via-in-pad samples, because solder wicking changed the pad impedance.

Three practical rules have saved me more than any solver setting. First, put ground vias tight around every signal via, within roughly a tenth of a wavelength, and keep the ground return continuous through the transition; a signal via with a distant ground return is an inductor, whatever its type. Second, keep the stub under 0.2 mm, or back-drill it, and model the antipad clearance as actually etched, because a 0.1 mm error in antipad diameter moves the resonance noticeably. Third, qualify the fill: ask the board shop for cross-sections, check for voids, and X-ray a sample after reflow. A voided or unfilled via-in-pad is worse than a careful dogbone.

For measurement, compare the transitions on the same coupon, de-embedded with a through-reflect-line kit, over the full 24 to 32 GHz band rather than at 28 GHz alone, and repeat after reflow and after a thermal cycle. If the return loss degrades after reflow, suspect solder in the via or a pad lifting, not the simulation.
R Member
Question: how sensitive is this to temperature? Any thermal test data?
L Admin
@RF_Bench_Notes 「先看 stub,再谈 via 类型」这句该进 28 GHz 布线门禁:带残桩的通孔就是带内谐振器;换层用盲孔/堆叠微孔,出 BGA 用填孔盖帽 VIP,和你们 coupon 上 VIP 比 dogbone+通孔少 0.2–0.4 dB IL、回损好 5–8 dB 的趋势也对得上。

编辑部对齐三条实操:
1) 信号 via 周围地 via 约 λ/10 内,回流连续;远处地回流再漂亮的 via 类型也是电感。
2) stub <0.2 mm 或背钻,antipad 按实蚀刻建模。
3) 填孔要验收:切片/空洞、回流后 X-ray;空心或未填 VIP 往往比认真做的 dogbone 更差。

欢迎贴:板厂填孔空洞率、回流前后 VIP 变化,以及你们禁止「28 GHz 信号走通孔留 stub」写进哪份规范。

— rfforum 编辑部 / Editorial Team
广告 AdRenesas 瑞萨微控制器芯片产品照片Renesas Electronics微控制器、模拟与射频/时钟方案 · MCUs, analog, RF and timing访问官网 →免费展示 · 资料来自公开信息 · 如需撤下请联系 ads@rfforum.com
广告 Ad广告位招商 / Advertise hereads@rfforum.com · 刊例 Rate cardT2 · 728×90
Log in or register to reply.