# need 7pF to 10pF at 2.5GHz

1. ## need 7pF to 10pF at 2.5GHz

i need 7pF to 10pF capacitor at microwave frequency or 2.5GHz. This is for PCB implementation. so any SMT capacitors parts or PCB capacitor implementations are welcomed.

•

2. ## [ADS] need capacitor with value of 7pF to 10pF at 2.5GHz

i need 7pF to 10pF capacitor at microwave frequency or 2.5GHz. This is for PCB implementation. so any SMT capacitors parts or PCB capacitor implementations are welcomed.

i have tried combining SMT capacitors in parallel but the capacitance is not flat enough at the frequency of interest (2.3GHz - 2.6GHz).

for your information, im designing using ADS. interdigital cap is available in ADS but the max value it can go is 1pF.

any other method to solve this problem is welcomed.

3. ## Re: [ADS] need capacitor with value of 7pF to 10pF at 2.5GHz

"capacitance is not flat enough" should be read as operating the capacitor near the SRF respectively parasitic package inductance being too large. Variation of the inner capacitance itself can be probably neglected in the 2.5 GHz range.

Package inductance is mainly defined by the package form factor and can't be reduced at will. I expect that PCB trace inductance is even a much bigger problem at the designed impedance level of about 6 ohms. But if you are really working in this range and have the PCB impedances correctly calculated, multiple small parallel MLCCs of 0201 size (or smaller) should work for you.

1 members found this post helpful.

4. ## Re: [ADS] need capacitor with value of 7pF to 10pF at 2.5GHz

Originally Posted by FvM
But if you are really working in this range and have the PCB impedances correctly calculated, multiple small parallel MLCCs of 0201 size (or smaller) should work for you.
Good point, the low impedance is the issue. Series inductance from the physical size then quickly changes everything. I used the Murata library to get the effective series capacitance for a 8.5pF SMD in 201 size, Murata type GRM0335.

In a real circuit, shrinking the cap size might not help if you still have the routing trace length. Even with EM simulation, it will be difficult to be that precise in simulating all the physical dimensions.

1 members found this post helpful.

5. ## Re: need 7pF to 10pF at 2.5GHz

Just about any small (0201, 0402) should be more than adequate at 2.5GHz. Do you have any other requirements? Voltage? ESR? ESL?

For example:
https://www.mouser.com/datasheet/2/2...MD-1101233.pdf

1 members found this post helpful.

6. ## Re: [ADS] need capacitor with value of 7pF to 10pF at 2.5GHz

Originally Posted by FvM
Package inductance is mainly defined by the package form factor and can't be reduced at will.
package inductance will be small for smaller size capacitors?

- - - Updated - - -

Originally Posted by FvM
Package inductance is mainly defined by the package form factor and can't be reduced at will.
rhanks for the answers.

- - - Updated - - -

im working on 1005 capacitor now as 0201 doesnt work for me. thanks FvM and Dr Volker.

- - - Updated - - -

Originally Posted by FvM
I expect that PCB trace inductance is even a much bigger problem at the designed impedance level of about 6 ohms.
Usually, i design RF traces (interconnects) to 50ohm characteristics impedance. for 2.5GHz, trace characteristic impedance have to be 6ohms instead?

- - - Updated - - -

Originally Posted by FvM
But if you are really working in this range and have the PCB impedances correctly calculated, multiple small parallel MLCCs of 0201 size (or smaller) should work for you.
im designing mixed element (lumped and distributed element) bandpass filter at 2.5GHz. so far multiple capacitor doesnt work. i tried 0201 size cap as well and tried it on circuit without interconnect/traces.

7. ## Re: [ADS] need capacitor with value of 7pF to 10pF at 2.5GHz

Originally Posted by barry
Just about any small (0201, 0402) should be more than adequate at 2.5GHz.
That's what I was thinking - until I looked at the actual data. The issue is the value used here. For such large C with small X, the series inductance becomes relevant even at low GHz. The PDF that you attached also shows the effect - look at SRF of the 7-10pF caps.

Originally Posted by pragash
Usually, i design RF traces (interconnects) to 50ohm characteristics impedance. for 2.5GHz, trace characteristic impedance have to be 6ohms instead?
No, he meant that every length of interconnect will have inductance, and matters at these low impedance levels. At the internal nodes inside your circuit/filters, you don't have 50 Ohm impedance levels. The 50 ohm is between the circuit blocks.

8. ## Re: [ADS] need capacitor with value of 7pF to 10pF at 2.5GHz

Originally Posted by volker@muehlhaus
That's what I was thinking - until I looked at the actual data. The issue is the value used here. For such large C with small X, the series inductance becomes relevant even at low GHz. The PDF that you attached also shows the effect - look at SRF of the 7-10pF caps.
.
agreed.one of the way is to stack up capacitors in parallel but in my case, it didnt work even after combining 7 to 8 capacitors.

- - - Updated - - -

Originally Posted by volker@muehlhaus
No, he meant that every length of interconnect will have inductance and matters at these low impedance levels. At the internal nodes inside your circuit/filters, you don't have 50 Ohm impedance levels. The 50 ohm is between the circuit blocks.
Thanks for the explanation. The impedance of the interconnect between components (within a filter) doesn't matter if the length of the interconnect is less than 1/20 of lambda. losses due to mismatch reflection of the interconnect are neglected because it's very small.

but i agree every length of the interconnect will have inductance. however, if we increase the interconnect thickness, we can reduce this inductance significantly. shorter and thicker traces are preferred for low inductance.

Please share your point of view on my comments.

If you have any guideline to do filter PCB layout for 2.5GHz, please share. thank you so much.

9. ## Re: need 7pF to 10pF at 2.5GHz

The impedance of the interconnect between components (within a filter) doesn't matter if the length of the interconnect is less than 1/20 of lambda.
No, the impedance generally matters, but it can be analyzed as lumped series inductance and parallel capacitance.

ADS can design the filter including all parasitic impedances, both interconnects and components.

1 members found this post helpful.

10. ## Re: need 7pF to 10pF at 2.5GHz

any guideline on the characteristic impedance of the interconnects? what is the optimum value of interconnect characteristic impedance for minimum parasitics inductance?

•

11. ## Re: [ADS] need capacitor with value of 7pF to 10pF at 2.5GHz

Originally Posted by pragash
but i agree every length of the interconnect will have inductance. however, if we increase the interconnect thickness, we can reduce this inductance significantly. shorter and thicker traces are preferred for low inductance.
I doubt that PCB trace plating thickness has a relevant effect on trace inductance. Or maybe you meant width, then I agree. The main rule is: make it short.

Or even better: if you can't avoid interconnect length, make that interconnect part of your design. It adds series inductance, so use a filter structure where that series inductance doesn't damage the response, or possibly improves it.

What filter type do you need to design (filter specs)? What are the PCB space restrictions?

1 members found this post helpful.

12. ## Re: [ADS] need capacitor with value of 7pF to 10pF at 2.5GHz

Originally Posted by volker@muehlhaus
I doubt that PCB trace plating thickness has a relevant effect on trace inductance. Or maybe you meant width, then I agree. The main rule is: make it short.
sorry for being not clear. yes , it is width.

- - - Updated - - -

Originally Posted by volker@muehlhaus

Or even better: if you can't avoid interconnect length, make that interconnect part of your design. It adds series inductance, so use a filter structure where that series inductance doesn't damage the response, or possibly improves it.
actually, i did this already and its meeting the specs. my only worry now is the correlation between simulation and measurement. having variable inductors as interconnects (varying the thickness of each interconnects) means I cannot optimize the design during measurement incase if my simulation does not correlate with the measurement. i cannot optimize meaning, i will have limited choice of lumped components to safe my design incase if simulation does not coreelate with the measurement. since each interconnect thickness is unique, the simulation have to corelate with the measurement. i worried its a one way ticket. thats why i prefer uniform interconnect but its seems impossible..

- - - Updated - - -

Originally Posted by volker@muehlhaus

What filter type do you need to design (filter specs)? What are the PCB space restrictions?
I'm designing small ISM band bandpass filter (2.4GHz - 2.5GHz) filter with two transmission zeros and sharp cut off. it's a discrete design so the only way is to use lumped components or mixed elements (lumped components and distributed elements). distributed element filter (coupled line and etc) is too big for this application. lumped components alone is impossible due to unavailablilty of microwave capacitance and unique value of inductance.

- - - Updated - - -

if you have any filter topology will work for PCB application, please do suggest.

- - - Updated - - -

Originally Posted by volker@muehlhaus

Or even better: if you can't avoid interconnect length, make that interconnect part of your design. It adds series inductance, so use a filter structure where that series inductance doesn't damage the response, or possibly improves it.
if you have any success story in this, please let me know. i already have working design. i may attempt to do this.

13. ## Re: need 7pF to 10pF at 2.5GHz

I meant to absorb parasitic series L of capacitor + routing into the surrounding components, but of course that depends on the actual circuit topology.

14. ## Re: need 7pF to 10pF at 2.5GHz

Looks feasible for a lowpass. Bandpass with the requested parameters is less pleasant.

15. ## Re: need 7pF to 10pF at 2.5GHz

this parallel resonance circuit is part of the filter. I tried to replace capacitor (with interdigital cap) and inductor (spiral inductor) independently but failed. it's not replaceable by lumped element or distributed element independently. any idea to convert this to parallel resonant circuit? open or short stub is too large so not preferred. Preferablly small form factor.

16. ## Re: need 7pF to 10pF at 2.5GHz

Have you considered using an LTCC band pass filter?

https://www.digikey.de/product-detai...1-1-ND/1560910

1 members found this post helpful.

17. ## Re: need 7pF to 10pF at 2.5GHz

hi Volker,
I'm designing it. thanks for the suggestion anyway. i learned a lot by designing it. one of the lessons is negative inductance is not bad at all for the spiral inductor. we can still design low loss/high Q negative inductor based on ADS simulation.

18. ## Re: need 7pF to 10pF at 2.5GHz

Originally Posted by pragash
I'm designing it.
You are designing in LTCC technology?
Then I don't understand your question regarding SMD, because you have so much more options to create "printed" components in LTCC.

Originally Posted by pragash
one of the lessons is negative inductance is not bad at all for the spiral inductor. we can still design low loss/high Q negative inductor based on ADS simulation.
I think you need to be careful with that, because you are then in a region with strong frequency depence where small tolerances can shift everything by a large amount.

•

19. ## Re: need 7pF to 10pF at 2.5GHz

Originally Posted by volker@muehlhaus
You are designing in LTCC technology?
Then I don't understand your question regarding SMD, because you have so much more options to create "printed" components in LTCC.
no, I'm not designing in LTCC. so far I have only done PCB circuit design and never has done LTCC design before. sorry to confuse you again :)

- - - Updated - - -

Originally Posted by volker@muehlhaus

I think you need to be careful with that because you are then in a region with strong frequency dependence where small tolerances can shift everything by a large amount.
I completely agree with that statement.

- - - Updated - - -

just wondering, how to do LTCC design? which software to use and etc? just curious.. might learn in future :)

- - - Updated - - -

there are high-frequency capacitors available from Murata. just sharing for the benefit of others.

https://www.murata.com/en-us/products/capacitor/slmc

20. ## Re: need 7pF to 10pF at 2.5GHz

LTCC is ceramic multilayer. I thought that the LTCC BPF from post #16 might solve your design problem, it is small (2,00mm x 1,25mm) and cheap.

Long ago I supported an LTCC manufacturer (Epcos TDK) with their filter designs for mobile phone front ends. It was lumped circuit design, transformed to layout elements, with heavy use of EM. I have attached a little paper written by a colleague back then.

MWEE_JuneJuly03.pdf

A 2.4 GHz band pass in LTCC might look like this (4mm x 4mm)

and the schematic is this:

2 members found this post helpful.

--[[ ]]--