LC lumped components filter

cost difference fr4 and nelco 4000-13

Hi,

Can i ask you experts here, if i am designing a high pass filter using 0402 chip LC components; and i need a 4 layers PCB. Because my circuit consists some microstrip lines, i used the second layer as ground plane, with substrate height being 200um, thus forming microstrip on top layer and ground on second layer. The other layers 3, 4 are left unused.

From you experience how much clearance does the ground plane need to be away from the lumped components located on top layer? Will ground plane cause problems when it is 200um away from the components?

My measurement results show the filter shape has shifted by down by 100MHz lower than desired (ie 800MHz instead 900MHz). Can you suggest why it shifts to lower frequency, any possible causes?

Many thanks

lc filter with parasitics

The frequency of the filter shifted 100MHz down from the reason of thin PCB layer 200um and higher parasitics. To get the right results you have to input in your simulator all these higher parasitics.

The problem with thin substarte is that you get very thin 50 ohms transmission lines (not very good for volume production, due to PCB manufacturer tolerance). You have to place the ground layer one layer below (at 400um) from the TL.

lumped lc filter

The main parasitic parameter is probably pad capacitance, it should be considered in an exact calculation or empirical corrected dimenioning anyway. But it could be expected almost reproducable, thus it isn't actually a problem. The strip line impedance probably is, as mentioned.

stacked lc filter

Is your PCB material FR4? FR4 material is extremely inconsistent in its dielectric constant. Also, it's stacked layer thickness varies from different vendors.

lc lumped t circuit

yea its FR4, thank you very much for all your suggestions.

I measured a linewidth, it was 378um, which is close to simulations of 50 ohm. But the actual measurements on Smith Chart, the impedance is below centre point and the line is capacitive. The line consists of pads as you mentioned.


But do you think ground plane clearance is required for LC components? if so, is there a rule of thumb, for example, ground plane should be at least 500um away from the 0402 chip components? i am in a bit of hurry so i have no time to replicate now and need to submit my report...but many thanks for you guys....

Any more suggestions, welcomed.........

Dear mchpddl1,

Having 100 MHz down shift is absolutely normal for such situation. The major reason usually is components parasitic, not the board. But you use so bad material that it is also contributes a lot to you down shift. I believe that if you switch from FR4 to Nelco 4000-13 or similar substrate (GE have some good) AND remove the ground plane under the pads with 10% margin you will get much better results. Nelco 4000-13 has about the same cost as FR4 but much better parameters and stable Er=3.7 and tanD=0.008 up to 10 GHz. Let me know if you need the datasheet for Nelco substrate.

The best and fastest solution is to design your filter with Genesys and then simulate it with Genesys' Empower EM simulator. Usually result is about 10 to 20% downshifted. Then redesign your filter with the same shift as EM simulation showed but in opposite direction (shifted up). Usually one such iteration is enough to get right first pass design. What is very important is to keep all the connections in the filter circuit as short as it possible and simulate it with the actual connection lines. If you have no Genesys you may use LINC2. Although it is inexpensive linear simulator it has excellent physical transmission lines models and I always use it before Genesys because it is much faster, but provides very close results without bulky EM simulations. The width of filter's short inside connection lines should be equal to component pads width, rather than to system characteristic impedance (usually 50 Ohm).

I hope it helps.

I do not know how to express but thank you very much for your experienced suggestions. i will propose what we should do next in the report, and hopefully we will compensate the shift as yuo mentioned.

Thanks once again mate.

You are welcome! Please let me know if you need something else. I am not sure about my schedule and may be not able to check EDA site every day, so, if you posted the question and I am not responded quickly please use pm.