SMD pad thicker than trace

[Nikos A.]

Hi every one, I design a RF pcb. I want to use 1608(metric) components but their size is much bigger than my trace width.

Is this an issue that should take into consideration? If yes, how should I manipulate it?

Thanks in advance

Nick

[Psi]

Shouldn't cause a problem.
But remember to use thermal relief

[wraper]

Where you ever seen pads that are of the same size as trace width to begin with?

[langwadt]

Where you ever seen pads that are of the same size as trace width to begin with?

with wide traces needed for impedance control or current?

[T3sl4co1l]

Well, in sufficiently small components (0201?), you'll get the same width.  Or in thick substrates with wide trace width.

If you can't afford the lower TL impedance of a wide component for whatever length it has, you can adjust to a certain extent by thinning the connecting traces (this makes a matched impedance lowpass filter), or adjust by removing ground plane underneath the component (so the height above ground is locally higher, proportional to the width of the component).  Obviously the latter only works if you have other layers in the PCB stackup that can be set to ground, and stitched to the main ground.

This is unlikely to be a problem because the key is found in the above analysis: the length of the discontinuity is the length of the component and pads.  That gives a frequency pole on the order of the 1/4 wave frequency, or for a 0603(1608) part, 31GHz.

At frequencies below, say, 6GHz, you have no problem whatsoever.

Tim

[Nikos A.]

Thank you all for your answers!! The frequency will be below 3Ghz..

But remember to use thermal relief

This is due to the 1608 size?

[Nikos A.]

One more question.. Can I use test points for across RF signal traces? Is it a good practice or it going to degrade the performance?

[DaJMasta]

Easiest way to do test points is an extra DC blocking cap or zero ohm jumper that can be inserted into the signal path (diverting it) to an RF connector.  That way you can switch the orientation of a passive and get the signal at the next stage on your output connector without excessive inductance or loading.  You could also use a bit of microstrip on the PCB parallel to a trace as a coupler that you terminate into a 50 ohm load, then just take your measurements from that.  Doesn't give you the level of the signal, but you could calculate the level based on the level the coupler picks up, and gives you the waveform just fine.  Since the microstrip would normally be present and terminated in the functioning design, probing it with a termination in your measurement equipment means the circuit under test isn't seeing any different loading, though it does mean that power coupled into it is wasted when the design is operating normally.


Test points work just fine for bias voltages and such, though, and you can also use EMI probes or other antennas to take a look without designing in other features.

[E Kafeman]

Freq is below 3 GHz, so I assume it is above 2 GHz.
In general if RF base frequency is above 2 GHz is 0603 a bit unusual big in size in my opinion if it is for consumer electronic.

Resulting signal function can vary a lot, not directly due to pad size but due to selected component size which affects pad size.
When building a copy of an RF radio application example: By manufacturer provided PCB design and BOM can not be adjusted and still expect same result.

For small capacitors, say 1-2 pF (as well as inductors) can stray capacitance be big part of component impedance at 2.4GHz and higher. Stray capacitance is much related to total body surface area.
In most cases are stray losses not critical for function but degrades filter functions and can cause a tuned circuit to become untuned.

A inductor, say 10nH at 2 GHz, can differ a lot in behavior  depending on if selected size is 0603 or 0402. Especially if it is a design that require low losses and high Q as SFR can be as low as 5-6GHz.
A common problem is harmonics around 5 GHz and upward. Amount of not suppressed harmonics can differ a lot depending on which type and size of components that are selected even if stated reactive value is same.

As an example, S-curve for a 10nH 0603 wire wound coil of Murata or Coilcraft brand at 5GHz differs as night and day and because of this can doing the right selection of brand be critical if function is to suppress BT harmonics in range 4.8-5 GHz, FCC fail or not fail.
A value of 10nH is maybe a extremely high value at 5 GHz but sometimes does it come in play unusual ways such as a part of base band filtering and Tx biasing at 2.4GHz and will then also affect higher frequencies.

Most professional filter simulation software allows to switch between different component types such as film relative wire wound type of inductors, sizes and different brands to cover these non ideal differences.
Capacitors are more friendly and similar between different brands at these frequencies. Stray losses and ground losses due to less stable RF ground are among the more common problems related to capacitors in RF circuits that I have seen.

In my designs, BOM is a law. If customers selects another brand of components or other sizes of same component family is that not any longer a design that I am responsible for.

Whenever you design or select component values, at least for most common SMD inductors and capacitors, is it very easy to check S-parameters. All manufactures have them for download.
These results are often measured under very good circumstances so that PCB losses or stray losses affect result minimal so when checking SFR (self resonance frequency) add margins for your design.
SFR is the frequency where an inductor not any longer is an inductor, it becomes an capacitor.

[Nusa]

Thank you all for your answers!! The frequency will be below 3Ghz..

But remember to use thermal relief

This is due to the 1608 size?

The thermal relief is so you can solder something to the pad in a reasonable amount of time. Otherwise, a fully connected large trace or layer will steal so much heat that you have to heat up a lot of the board to accomplish the task.

[Nikos A.]

Thank you very much for your answers!!

E Kafeman, your post was really helpfull!!

Do you have to suggest any RF simulator software that you use?

[E Kafeman]

There are many software that can handle components and PCB at S-parameter level and doing PCB RF analyze.
They are way to expensive for the normal hobbyist and can do much more then analyzing components and pads sizes:
A rather simple software can else be Microwave Office. There is a free trial here but do not know how free it is: https://www.awrcorp.com/download-ni-awr-design-environment
It is still a lot of fiddling with "black boxe simulation" for each type and value of reactive components or parts of PCB traces.

A easy way comparing difference between component types and brands can this software be worth checking: https://www.atyune.com/
Free for long time..

A different group of software, more of a lab bench tool then simulator is AnTune.
Professional and only of use if your own IEEE-488 compatible VNA conneted to a PC.
Free for a limited period.
It use a VNA to measure an existing empty PCB trace pattern (or anything measurable with a VNA such as a PCB embedded antenna) and allows you to add or switch between real and simulated component and topologies for the most common types and brands of reactive components or let software automatically select to find most lossless component selection and topology for impedance match between two ports.
Can however not recommend this software as it could be seen as self advertising.

Recommend alternative software doing somewhat same things as AnTune:
http://www.mnw-scan.com/index.html
https://www.optenni.com/

[Nikos A.]

Thank you!!