The backdrill process removes stubs from plated-through-holes (vias). Stubs are the unnecessary / unused portions of vias, which extend further than the last connected inner layer.
Stubs can lead to reflections, as well as disturbances of capacity, inductivity and impedance. This discontinuity errors become critical with increasing propagation speed.
Backplanes and thick Printed Circuit Boards in particular, can endure significant signal integrity disturbances through stubs. For High Frequency PCBs (e.g. with Impedance control), the application of backdrilling, as well as the application of blind and buried vias, can be part of the solution.
Backdrill can be applied to any type of circuit board where stubs cause signal integrity degradation, with minimal design and layout considerations. In contrast, when using blind vias, the aspect ratio has to be kept in mind.
Advantages of Backdrill:
- Reduced deterministic jitter
- Lower bit error rate (BER)
- Less signal attenuation with improved impedance matching
- Increased channel bandwidth
- Increased data rates
- Reduced EMI radiation from the stubs
- Reduced excitation of resonance modes
- Reduced via-to-via crosstalk
- Aspect ratio can be neglected (in contrast to blind vias)
Send us an additional info layer in your production data, identifying the vias intended for backdrilling. Different backdrill depths can, for example, be identified through different symbols in the info layer. Please contact us, we are happy to help!
Design Parameters
| Index | Type | Value min. |
|---|---|---|
| A | Backdrill Ø | 400µm |
| B | Plated-through via Ø | 200µm |
| C | Copper clearance | 150µm |
| D | Ø-Difference circumf. | 100µm |
| E | Backdrill depth | 200µm |
| F | Distance to connected layer | see below |
| G | Thickness target layer | see below |
| H | Thickness stub remainder (safety) | see below |
Required target layer thickness "G"
If you need a special layer buildup, please keep to the following min. prepreg thickness of the layer in which the drilling stops (G).
If you do not need a special layer buildup, we will do all the necessary thickness calculations regarding the thickness of "G".
| G min. | 250µm | 300µm | 400µm | 500µm |
|---|---|---|---|---|
| H | 125µm | 150µm | 200µm | 250µm |
| Tolerance | ± 100µm | ± 125µm | ± 175µm | ± 225µm |
Stubs in Detail
As already mentioned, stubs interfere with the signal integrity of high-frequency circuit boards. Stubs cause unwanted resonant frequency nulls which appear in the insertion loss plot of the channel.
If one of these frequency nulls happen to randomly line up at or near the Nyquist frequency of the bit rate, it will result in a high bit-error-rate; even link failure. The shorter the stub, the lower is the probability of error.
For simulating stubs, as well as high-speed digital design layouts, the software ADS by Keysight Technologies can be used. ADS is capable of linear, non-linear and electromagnetic (2.5D and 3D) simulation. Keysight is internationally - practically to any extent - with its many years of experience and the exclusive focus on measuring technology one step ahead.
Graphic "insertion loss" kindly provided by Bert Simonovich - Design Notes on Stubs.
Deeper into the matter: Stub Termination