LC filter using Air Core Inductor Interesting Transfer Function

[Glenn0010]

Hi All,

I'm doing an analysis of a simple LC filter using an Air Core Inductor. I'm getting an interesting transfer function.

I'm simulating the air core inductor using Ansys Q3D and then importing the model into Ansys Simplorer (essentially spice) to simulate the bode plot.

Here is the Q3D model. Inductance of roughly 1uH, AC resistance of about 2R at HF, Inductor capacitance of around 2 pF (I'm pretty sure this is referring to capacitance between source and sink)


I then go to simplorer to compare against an ideal LC filter


This is the bode plot. The green plot shows that after ~200 MHz the attenuation increases to 80 dB/dec. The inductor end to end capacitance would cause this attenuation to reduce not increase so it can't be that. I've checked in a transient simulation and the self resonant point of the air core inductor is roughly at this frequency. So what is causing this additional attenuation after the self resonant point? At 80 dB/dec, this means that 2 additional energy storage elements are there. But I'm struggling to come up with an equivalent model that reflects this. My best guess atm is that it is magnetic and capacitive coupling between adjacent segments but how do I model this electrically? Another option would be proximity effect however would this be a sudden change in attenuation?



Any help is much appreciated

[mawyatt]

What are the R and C values in the schematic?

Plots look like you have 2 resonances, first at ~1.5MHz and second at ~250MHz. The "Q" of the first is reasonable, the second looks like a very high "Q" due to the phase transition.

Apparently the first resonance is due to the lumped element inductance, the second is likely due to another distributed field resonance since the "Q" is so pronounced. The FR4 will increase the interwinding coupling capacitance which may have an effect, try removing the FR4 and re-simulate to see what the effects are.

Also, this second resonance could be to due to an artifact created by the 3D Modeling. Do you have access to the actual model parameters used in the plot simulations, or is this a "Black Box" treatment for the inductor?

Best,

[Glenn0010]

Hi,

The capactiro value is 10 nF and the load resistor is 1k. So that explains the first resonant point and the Q factor is not great due to the skin effect of the inductor of about 2 ohms so that all matches.

I've tried removing both the air and fr4 and very little difference was done, so it doesn't look like it's that.

I'm also thinking its due to some distributed component and its seems to match the resonant frequency of the inductor but am not sure how that increases attenuation

I'm not sure what you mean by access to the model parameters, but I drew the inductor on Inventor and the imported it onto q3d. Wire is 3x0.75 mm copper. So I can adjust dimensions and so forth. Pitch between windings is 2 mm. I'm wondering how I could check wether it's an artifact in the simulation.
Thanks

Glenn

[mawyatt]

Wondering what the model the 3D field simulator creates looks like? If it's "SPICE" compatible this might give some clues about the 2nd resonance.

The 3D simulation artifacts could be due to various parameters used to create the model. We don't have experience with Ansys Q3D but older 3D Field simulators had various user tweakable parameters to assist in achieving a respectable and realistic result.

Best,

[Benta]

The second peak could be a standing wave resonance, where the coil length corresponds to 1/2 wavelength at 250 MHz and the trace is working as a transmission line.
Happens when input and output is not impedance matched.
Try making the inductor physically smaller (= shorter trace length) and see if the peak moves higher in frequency.

[Glenn0010]

Hi All,

I'll try your suggestions after the weekend as I'm away currently.


I'm wondering even if there's a standing wave, at the second resonant point, how would this cause the attenuation increase at higher frequencies?

Thanks

Glenn

[T3sl4co1l]

Not sure offhand how the simulator is going to handle common mode, or what outer boundary conditions, or properties of the ports, you've set.  But evidently you have power going somewhere else; a one-port cannot have more than 180° of phase shift, but apparently you have 360.  I assume that's going into the radiation "port".

In general, inductors are transmission line components: they're made of wire, and wires beside wires make transmission lines, and transmission lines have various order resonances.  So we expect to see higher order modes, typically at frequencies harmonic to the winding electrical length, but give or take geometric factors, what's in the space around it (core), etc.  For example, a solenoid (helix) winding can be modeled as a helical waveguide, which has dispersive modes (Zo rises and velocity falls as frequency goes up ...I think?!).

The first peak in the transfer function is the expected LC resonance; the peak comes down with source/load resistance.  The later peak must be the inductor's series resonance, which will be around the 1/2 wave point of the spiral.

Tim

[niconiconi]

The inductor end to end capacitance would cause this attenuation to reduce not increase so it can't be that. [...] I'm struggling to come up with an equivalent model that reflects this. My best guess atm is that it is magnetic and capacitive coupling between adjacent segments but how do I model this electrically? Another option would be proximity effect however would this be a sudden change in attenuation?

I can't comment on the simulation, but I'd like to point out that realistic inductors cannot be modeled by simple interwinding or end-to-end capacitances. The full physics is rather complicated that involves both the theories of helical RF resonators and transmission lines. There are many engineering models but all are approximations, nothing captures the full-range of behaviors (which is why people use field solvers). The general case is arguably still an open research problem.

For more information, see:

The self-resonance and self-capacitance of solenoid coils:
applicable theory, models and calculation methods.
By David W Knight

https://g3ynh.info/zdocs/magnetics/appendix/self_res/self-res.pdf

[Glenn0010]

Hi All thanks for your feedback,

I guess even such a "simple" geometry is not so simple to model.

I've plotted the surface current density in the inductor. Here you can see there are "cold" spots across the inductor. Is this indicating that there is the standing wave as you folks have suggested where the cold spots are the points that are 0 magnitude in the sanding wave? Is my interpretation of that correct?



I've also plotted the magnetic fields here. Not really sure what to make of them. They seem to make sense to me.  Top view
,

Across there inductor here
,

Cheers Glenn

[T3sl4co1l]

Hmm neat, is that a 3/4 wave condition?  Or wait, what's the exact winding length halfway point? The spiraling is fairly strong here, worth checking.

I've also plotted the magnetic fields here. Not really sure what to make of them. They seem to make sense to me.  Top view

Try plotting it as Z axis component (signed), rather than magnitude.

Tim

[Glenn0010]

Hi, Teslacoil

So I've calculated the length of the coil (good call!)  The half way point is somewhere in the segment where one of the cold spots is


I've also plotted the z axis magnetic field signed as you suggested.



This is all cool and I'm learning the software and more about HF behaviour.

However it's still not obvious to me as to why after the self resonant point the attenuation increases.

Cheers

Glenn

[mawyatt]

However it's still not obvious to me as to why after the self resonant point the attenuation increases.

Cheers

Glenn

Not sure if this is what you are referring too.

If you look at a resonate structure mathematically and take the derivative of the "Impedance" vs frequency you'll find this rate of change is unbounded when the resonate "Q" approaches infinity.

What this means as the impedance magnitude reaches extremes at resonance, the rate as approaching resonance from either frequency direction can be quite high. If the network under consideration is a filter with resonate devices then the filter attenuation "skirts" can be quite high with high "Q" resonate devices.

A good example is a quartz crystal, look at the impedance plots that go from series resonance (low Z) to parallel resonance (high Z), and note the rate of change approaching the series and parallel resonances. Below is an example of a 32.768KHz we measured here:

https://www.eevblog.com/forum/index.php?action=dlattach;topic=370133.0;attach=2351981;image

Note the impedance ranges and rates of change of such with frequency.

Crystals are often utilized in bandpass filters which exhibit extremely high attenuation rate "skirts", these filters were often used in older communication receiver IF stages before DSP techniques came into play.

Best
 

[T3sl4co1l]

This transfer curve;



Basically, depends on how it's modeled, if it's including radiation in some form, there can be a common-mode port implicit and thus what you thought was a one-port is actually two and thus you're measuring not an impedance but a transfer function, and hence there's a path for that (reflection) current to flow to GND through.

Tim

[Sensorcat]

Since the data sheet of Ansys Q3D does not mention radiation, I think it is safe to assume that it is not modeled:

https://www.ansys.com/content/dam/amp/2022/may/asset-creation/q3d-extractor-datasheet/ansys-q3d-extractor-datasheet.pdf

OTOH, the description clearly tells that the program creates a SPICE model. So there must be such a model that is transferred from the FEM part of the simulator to the SPICE part, as shown by the OP. We need that model to find what's going on, even better together with the full netlist that is used in the SPICE simulation. It should be possible, since the data sheet mentions the possibility to transfer models to other SPICE simulators (table on page 1, last row).

Regarding the impossibility of 360° phase shift in this system: That's 'only' in reality, but some, if not many, simulation programs are sort of 'unaware' of the circularity of phase. So the user must take into account that 360° means the same as 0°, e.g. by applying the popular unwrap() function, if wanted (and available).

[mawyatt]

Since the data sheet of Ansys Q3D does not mention radiation, I think it is safe to assume that it is not modeled:

https://www.ansys.com/content/dam/amp/2022/may/asset-creation/q3d-extractor-datasheet/ansys-q3d-extractor-datasheet.pdf

OTOH, the description clearly tells that the program creates a SPICE model. So there must be such a model that is transferred from the FEM part of the simulator to the SPICE part, as shown by the OP. We need that model to find what's going on, even better together with the full netlist that is used in the SPICE simulation. It should be possible, since the data sheet mentions the possibility to transfer models to other SPICE simulators (table on page 1, last row).

Exactly, what we mentioned in post #3

Best,

[Glenn0010]

Buckle up, it's going to be a long one

Hi, so I've had a look at what you guys have suggested and acted on it, and have a few other things

So firstly here is the spice net list that it generates

Code: [Select]

.subckt HF_Filter_only 1 2
XZhalf1 1 3 HF_Filter_only_half
XY1 3 HF_Filter_only_parlel
XZhalf2 3 2 HF_Filter_only_half

.subckt HF_Filter_only_half 1 2
V1 1 3 dc 0.0
R1 3 4 1.02964304755
L1 4 2 4.85616143593e-07
.ends HF_Filter_only_half

.subckt HF_Filter_only_parlel 1
R1_0 1 0 58242.2291893
C1_0 1 0 1.99441172183e-12
.ends HF_Filter_only_parlel

.ends HF_Filter_only
So I looked at this and it and recreated it in simplorer. As I understand it, it basically splits the coil in 2 and added 2 pF cap to ground as below. (In the model I rounded the components to 500 nH per inductor and 2 pF for the cap).
We can see now that the bode plot matches. - So we know that there is a capacitance to ground... How??



So I pulled up the Ansys Q3D documentation mainly relating to capacitance. Basically the software models the capacitance of the inductor to ground at infinity. So that's what the 2 pF is as in the spice model. (I thought this would be the interwinding capacitance or something similar - wrong! - So I can't get the inter winding capacitance then?)



According to documentation another option is that I can float the coil at infinity.



So I simulated this using the FloatInfintyMatrix and the "Inductor, Inductor" capacaitance becomes 0 pF. So this confirms that it is capacitance just to ground as explained above.

The spice netlist now becomes as below. The same as before but without the capacitance shunt conductance to ground.

Code: [Select]

.subckt HF_Filter_only 1 2
XZhalf1 1 3 HF_Filter_only_half
XY1 3 HF_Filter_only_parlel
XZhalf2 3 2 HF_Filter_only_half

.subckt HF_Filter_only_half 1 2
V1 1 3 dc 0.0
R1 3 4 1.02964304755
L1 4 2 4.85616143593e-07
.ends HF_Filter_only_half

.subckt HF_Filter_only_parlel 1
.ends HF_Filter_only_parlel

.ends HF_Filter_only

Looking at the new simplorer setup now we have the orignal inductor with the orignal matrix (the spice equivalent as well) and the one with the float at infinity matrix.


Now, the float at infinity matrix perfectly matches the more ideal LC circuit characteristics.


So we figured it out! The only problem to me now is that these bode plots look to be a bit too ideal at HF - no reflections or capacitive or anything.

So I tried an alternate route. Using Q3D I can extract the S-parameters for the inductor only both with the original and floating matrix.

Here with the S parameters I see more what I'd expect, some signs of reflections and transmission lines. So therefore, I'd expect these to be represented in the bode plots. This is a correct assumption no?

So my questions at the end of this is.
1.Which one is more representative of reality? The original matrix or the float at infinity? I'm planning a physical test when the wire arrives.
2.These bode plots seem to be to ideal so is that defeating the purpose of  using this software anyways.
3. Can I use the S-parameters instead to model - real-world behaviour of the inductor/filter. I will try to import the s-parameters in spice and see if the overall bode plot of the LC filter then changes.

Any feedback is appreciated.

Cheers for reading it all if you have

[T3sl4co1l]

Yes, the s-params look better. In particular, you see transmission peaks corresponding to series (nλ/2) resonances, and valleys to antiresonance (or parallel resonant, (2n+1)λ/4 wave).  You see the amplitude of the peaks decreasing as frequency goes up, as the spiral becomes a better and better antenna at such frequencies.

I wonder if the simulation would be a bit better behaved with some nearby grounded metal, or say one terminal mounted to a ground plane, and then you can do a one-port measurement and extract the SPICE (there might be a s-param to SPICE model fitting function in there?).  You would then have a one-port to GND, so then go through and edit all references to '0' with the other terminal and you have a freely wired one-port (two terminal) component.

It might also return different results if you define one terminal as GND, without doing anything else (planes or whatever).

A more meaningful simulation would be placing it inside a metal box (i.e. defined as GND), and treating it as a two-port -- the transfer characteristic then is obvious and necessary to apply in the outer (filter) model.  You've basically been forced into this (it put in the branch to ground for you, whether you meant it to or not -- SPICE always has a default '0' available, regardless of SUBCKT level, so this is easily hidden away inside a model), might as well lean into and formalize it.

Note that the lumped-equivalent model is only valid up to some accuracy, over some frequency range.  This must be specified, to avoid generating a laundry-list of elements from the complete (10GHz!) s-param curve.  Usually only one or two resonances are included, and this is sufficient for say power electronics purposes (give or take EMI, but if you're simulating EMI, you're probably doing EMI wrong*), or most RF purposes as you mainly need to know SRF so as to avoid it at frequencies of interest.

*That "probably" might be tempered by the presence of ANSYS in the thread, where whole-product wave, or even multiphysics, simulations are possible.  I don't know if that's part of your goal here, but suffice it to say, you're equipped to do so if need be, and given enough time to develop the models...

Tim

[Glenn0010]

Hi Teslacoil,

I think the next step now is to simulate the inductor in box as I was planning to put some shielding around it anyways. Then I'll see if I can use the s parameters for simulation in the simplorer (spice).

My goal here is to develop a filter and determine its frequency response (attenuation) up to 1 GHz. The filter design that I have in mind is more complex than the LC case I'm showing here but I thought I'd start with a simple case here.

I'm not sure how far I can get with Q3D but I think it might make decent starting point. I know another ansys package called HFSS is better for HF stuff but it's another tool to learn, so I though I'd stick with this one for now.

Cheers

Glenn

[Glenn0010]

Managed to import the s-parameters into simplorer. Here are the s-parameters of the inductor by itself plotted with more points for better accuracy


Here is the frequency response of the filter. We can see here that the s-params have clearly degraded performance vs the lumped parameters. This gives me more hope that the frequency response here is more realistic.


Next step is to do it again with it wrapped in gnd and see what we get.

Any suggestions welcome.

[Glenn0010]

Hi - update and interesting results

I added a box (shield) around the inductor on 5 sides. Copper 0.07mm (2oz copper). I assigned the shield as GND.



The inductance dropped compared to previously. I imagine the magnetic field in the coil is generating eddy currents in the shield causing some flux cancelation to occur which reduces inductance?



Here we can see the magnetic field interacting with the shield. Looks like there is some leakage? Is this an artefact or shall I increase the thickness of the shield.



Looking at capacitance, now to ground we have about 3.3 pF of capacitance. This makes sense, to me, it's larger since the ground is no longer at infinity. So now the ground shouldn't be infinity but now is the shield


So now we can plot the frequency response. VM3 is and ideal LC filter, VM1 is the spice equivalent model, VM2 is the S-parameter



Here's the bode plot



What's interesting here is that I was expecting the s parameter model and the spice model to be somewhat similar.  Since now we have the grounded shield around the inductor I was expecting that capacitance to ground to occur and cause the -80 dB/ attenuation after the 2nd resoant point. But this is not what's happening. Maybe the Q3D GND and the simplorer GND are not linked somehow.

Any thoughts?

Cheers