Problem Simulating Noise Figure of Gm Cell (single Ended)

Dear Saj008,

Saj008 said:

Could anyone help me out regarding this?

Did you examine the DC operating point of your circuit? I believe the DC operating point results in a behavior that is not consistent with your expected result. I might suggest that there are two issues with your circuit topology that do not place the active devices in their desired saturated regions.

1. Your output port is defined as a 50 ohm port whose DC value is 0. With a value of 0, this will shut off your pmos device as it forces its vdd to 0 V. Hence, the only device connected to your input port that has any gain is the pmos device.

2. Your input source is a port whose DC value is defined as 600 mV. With the impedance of your node to which PORT0 is connected not defined as also 50 ohms, the DC value of the gate to the pmos device is not 600 mV, and in fact, will be twice 600 mV or 1.20 V - which exceeds the source voltage as the source of the pmos device (1V). Hence, your pmos device gate-source voltage is negative and it is also off.

To verify my hypothesis, I made a version of your circuit and performed a DC and NF analysis. The DC operating point results are annotated in the circuit in Figure 1 with the resulting Noise Figure plot in Figure 2. The DC operating point appears to confirm my two hypotheses and the Noise Figure result appears similar to what you observe (albeit with different values as my inverter device sizes and its PDK is totally different than yours. 

Hence, I believe you need to correct the input port DC voltage and add a AC coupling capacitor between your inverter output and output port to prevent it from shorting the output voltage to ground.

Let me know your thoughts Saj008. I hope this helps a little...

Shawn

Figure 1

Figure 1

Figure 2

Hi Shawn,

Thanks a lot for showing precisely my mistakes. I really appreciate your time & help.

Yeah, there are some fatal mistakes in my single ended design. I will work on it.

I also tried a differential Gm-Cell to simulate the noise figure. I need to have a low NF at around 1Hz. But I am getting too high NF (around 86dB) at low frequency (necessary photos attached).

Could you please comment on this if you have time?

Thanks a lot

Saj

Dear Saj008,

Saj008 said:

I also tried a differential Gm-Cell to simulate the noise figure. I need to have a low NF at around 1Hz. But I am getting too high NF (around 86dB) at low frequency (necessary photos attached).

Could you please comment on this if you have time?

A couple of comments...I don't know enough about your devices or your output load - both of which are important in a low noise application.

1. Do both your nmos and pmos devices have substrate tubs? For example, is your technology some version of an SOI process? It is not typical to have the nmos device in a separate tub as in most conventional MOS technologies the substrate of nmos devices are all connected to ground. Your schematic shows the substrate connection of M0 and M2 to a node other than ground.

2. From your schematic and the DC operating point information displayed, it appears your output resistors are each 10K. If you are aiming for a low noise amplifier, are you concerned about the impact of this rather high output resistance?

3. Did you mean to write your objective was a low noise figure at 1 Hz?  I don't know know what magnitude of noise figure you are trying to achieve at 1 Hz. However, MOS based amplifiers will have an inherently high amount of low frequency noise. They are not used in applications where low frequency noise must be minimized as their 1/f noise and other low frequency noise sources are high. Their low frequency noise sources can be highly variable with silicon processing and hence modeling their very low fequency noise well  poses a significant challenge.

4. Are you sure your models accurately capture the noise of the devices at 1 Hz? Typically, 1 Hz is the lowest frequency measured for device noise - hence even the measurement accuracy can be questioned.

Hence, I am not surprised your noise figure simulation at 1 Hz appears high.

Shawn

Hi Shawn,

Thank you so much for your insightful comments.

I want to use the above differential amplifier as a Gm-cell at the output of my passive mixer, where my input RFfreq= 1GHz and LO/Clk freq=1 GHz. So for a down-conversion mixer, am I not supposed to get 0Hz at the output? That's why I am interested to the NF at 0 or 1 Hz.

I have simulated and got the NF peak at 0Hz, 1GHz and 2 GHz (photo attached) after connecting my Gm-Cell (diff. amp)  to the passive mixer output.

a) Shouldn't I put output frequency range starting from 0 Hz in Pnoise analysis? (photo attached)

b) Or Should I look at the NF at 1GHz? (but my output frequency is 0 Hz at the Baseband).

c) at which frequency ultimately I have to look for my required NF?

I really appreciate your time & help

Thanks

Saj

Dear Saj008,

Saj008 said:

Thank you so much for your insightful comments.

Of course! Use try to help!! However, I'm not sure how "insightful" my comments are!!

Saj008 said:

I want to use the above differential amplifier as a Gm-cell at the output of my passive mixer, where my input RFfreq= 1GHz and LO/Clk freq=1 GHz. So for a down-conversion mixer, am I not supposed to get 0Hz at the output? That's why I am interested to the NF at 0 or 1 Hz.

Yes, you are correct - and now I understand why you are concerned with such very low frequency noise components. Low frequency noise components and their impact of the signal-to-noise (SNR) ratio of a "direct down conversion receiver" is a well known issue. When designing a direct down conversion receiver, it is a major design consideration and worth studying. However, the "0 Hz" you mention is not considered a "low frequency noise component" but must be compensated for as DC offsets can saturate amplifiers with high gain in the conversion path. Techniques to handle DC offsets, I/Q mismatch, and other impairments for direct conversion receivers iare outlined and discussed in the highly referenced 1997 paper by Razavi "Design Considerations for Direct-Conversion Receivers".

To minimize the low frequency noise (and DC mismatch) of the direct conversion receiver relatively large devices are used. However, there is a trade-off between their size and their noise/mismatch as the large devices will have a larger input capacitance - which will lower the bandwidth. For this reason, and the added noise of MOS devices over BJT devices, that MOS devices are often not the "best" choice for a direct conversion receiver...my opinion only!

Saj008 said:

a) Shouldn't I put output frequency range starting from 0 Hz in Pnoise analysis? (photo attached)

Saj008 said:

b) Or Should I look at the NF at 1GHz? (but my output frequency is 0 Hz at the Baseband).

Yes. The pnoise analysis should be performed over the low frequency range of the direct conversion receiver output. The pas analysis prior to the noise analysis, however, should use the RF center frequency used to down-convert the receiver input. A good reference for simulating direct down converter receivers is provided by Cadence on the Cadence On-line support site at URL:

https://support.cadence.com/apex/ArticleAttachmentPortal?id=a1Od0000000nTiyEAE&pageName=ArticleContent

Have you searched or seen this Saj008?

There is also an Adobe Portable format document at URL:

Spectre Circuit Simulator RF Analysis Theory -- Basic Reference Information - Basic Reference Information

You did not show the SpectreRF simulation settings you are using for your pss analysis, but please pay attention to the number of sidebands setting for the analysis as it must contain a sufficient number of sidebands to capture all the folding to baseband.

I hope the added comments and references are of some use Saj008!

Shawn

Hi Shawn

Thanks a lot for your detailed explanation and suggestions. These advice are significant input for solving my problem of high noise figure.

BTW, I can not download the document of your given link (any of the twos). It requires Host ID or LMS ID after logging in.

Appreciate you time.

Saj

Dear Saj008,

Saj008 said:

BTW, I can not download the document of your given link (any of the twos). It requires Host ID or LMS ID after logging in.

I would strongly suggest you consider obtaining a Cadence On-line support account as it contains many very relevant documents that I think you will find most useful - not to mention will address many of your questions.! Please check with whomever maintains your Cadence tools and that individual(s) will provide your site license ID. You will need that to create an account.  I think if you do not have an account, that is why you cannot access the links I provided.

Shawn

Hi Shawn,

Yes,  I will obviously do that.

Thanks for your help.

Regard

Saj