***性和非线性器件模型？

正确设置了第一个带有s参数仿真的原理图，以完成仿真。
设计很奇怪，因为一些组件值看起来不正确。
在漏极连接中，永远不应该有一个31欧姆的电阻。
虽然需要连接元件来正确配置晶体管，但不需要直流源进行线性模拟。
第二个原理图是晶体管的封装器件模型。
这在源上有断开的线，因此这将导致不正确的结果。
看起来您正在设备上进行s参数模拟，但没有任何偏差。
这也是不正确的。
对于任何模拟，晶体管的这种模型只有在所需的工作点完全偏置时才能工作。
在第三个原理图中，您似乎正在重复使用从第二个原理图生成的数据集结果作为设备模型。
如上所述，该模型没有偏差，并且在该数据集中记录的所有内容都是在该无效/非操作偏差点处的简单s参数。
您应该将晶体管的实际器件型号的符号放在第三个原理图中作为子网络，而不使用术语和使用端口。



     以下为原文

  The first schematic with the s-parameter simulation is set up correctly to complete the simulation. The design is strange though as some of the component values do not look right. You should never have a 31ohm resistor in the drain connection. The dc source are not needed to do linear simulation although the connecting elements are required to get the match for the transistor configured correctly.

The second schematic is the packaged device model for the transistor. This has a disconnected wire on the source so this will cause incorrect results. It also looks like you are doing an s-parameter simulation on the device but without any biasing. This is also incorrect. This model for the transistor will only work, for any simulation, if it is fully biased at the required operating point.

In the third schematic it looks like you are reusing the dataset results generated from the second schematic as the device model. As explained above this model is not biased and all that is being recorded in the dataset is simple s-parameters at this invalid/non-operational bias point. You should really be placing the symbol for the actual device model for the transistor, without the terms and using ports, as a subnetwork into the third schematic.

当您将任何原理图设计重用为ADS中另一个设计的一部分时，它由表示该部分的符号表示。
默认符号是一个带有适当引脚数的简单框，但它也可以是自定义符号，如果它是以这种方式构建的。
要将设计放在另一个原理图中，只需在主窗口中选择名称并将其放在原理图中即可拖动设计。



     以下为原文

  When you reuse any schematic design as part of another design in ADS it is represented by a symbol that represent that part. The default symbol is a simple box with the appropriate number of pins but it caould also be a custom symbol as show if it was built that way. To place a design in another schematic simply drag the design by selecting the name in the Main window and place it in the schematic.

如果您不清楚某些基本操作模式和ADS的使用，我建议您考虑以下ADS在线学习课程。
ADS 2009 Update 1快速入门课程 - 1小时入门自学电子学习课程。
ADS 2009 Update 1基础知识电子学习 - 5小时的讲座和演示以及额外的自定进度实验室练习manerials作为可打印的PDF下载。
两者都是自定进度的在线培训课程，对用户免费。
您需要做的就是完成安捷伦知识中心的注册。
这些相同课程的版本也适用于更多当前的ADS版本，ADS 2011＆amp;
ADS 2012.编辑：sdgrant于2013年5月27日下午2:17



     以下为原文

  If you are unclear on some of the basic operation modes and use of ADS may I recommend that you consider the following ADS eLearning Courses.
ADS 2009 Update 1 Quick Start Course - 1 hour introductory self-paced e-Learning course.
  ADS 2009 Update 1 Fundamentals e-Learning - 5 hours of lectures and demonstrations and additional self paced lab exercise manerials as printable PDF downloads.

Both are self-paced online training classes that are free to users. All you need to do is complete registration of the Agilent Knowledge Center.

Versions of these same courses are also available for more current ADS releases, ADS 2011 & ADS 2012.

Edited by: sdgrant on May 27, 2013 2:17 PM

sdgrant先生，我真的在学习ADS 2009时面临很大的困难，请指导我如何从简单的基础到高级学习，请告诉我先生的方式。
请在ADS 2009中显示从基础到高级版本的所有PDF文档。编辑：ADSProductManager于2013年5月28日上午10:33



     以下为原文

  sdgrant Sir,
                    Really I am facing very much difficulty in learning ADS 2009, please guide  me how to learn from simple basics to advanced ,please show me the way sir.  Please show all the PDF document from basics to advanced version in ADS 2009.

Edited by: ADSProductManager on May 28, 2013 10:33 AM

要迁移，sourceId：108288



     以下为原文

  to be migrated, sourceId: 108288

亲爱的先生，我设计了线性设备模型和非线性设备模型。
非线性到线性，非线性结果的结果差别不大于线性结果。正如你所说，我没有使用直流分析和偏置进行线性模拟，我使用了非线性器件模型的偏置。
我对线性和非线性模型有很多困惑。
据我所知，非线性器件模型用于测量IIP3，OIP3，P1dB压缩点，线性器件用于测量增益，噪声系数和稳定性。
我对它有疑问，我们可以使用非线性器件模型来测量增益，NF，稳定性，IIP3，OIP3，P1dB压缩，你能说清楚吗？
我还有一个疑问，为了制造，我们需要在最后将偏置连接到线性器件模型。
我要求你明确线性和非线性，他们正在使用的目的。我们需要得到线性和非线性模型的完全相同的结果，如果两个模型之间差别不大，是o.k.



     以下为原文

  Dear Sir,
               I have designed both linear device model and nonlinear device model. Little difference found in the results of nonlinear to linear, nonlinear results are little less than the linear results.As you told that I didn't use DC analysis and biasing for the linear simulation, and I used the biasing for the nonlinear device model. I am many confusions about the linear and nonlinear model. As I know , nonlinear device model is used for measurement of IIP3,OIP3 ,P1dB compression point, linear device is used for measuring for gain, noise figure and stability. I have doubt on it, can we use nonlinear device model for measuring gain, NF, stability, IIP3,OIP3, P1dB compression, can you make it clear this. I have one more doubt , for fabrication do we need to connect biasing to linear device model at the end. I request you to make clear about linear and non linear, what purpose they are using.Do we need to get the exactly same results for both linear and nonlinear models, if little difference between two models, is it o.k.

你真的不应该考虑这种情况是什么模型可以做什么样的测量。
它完全基于您使用的模拟器。
例如，IIP3，OIP3和P1dB压缩是大信号测量，电路的响应取决于输入信号的特性，即幅度，DC偏移等，并且这些可以使用谐波平衡模拟来完成。
噪声系数和稳定性通常是小信号测量，其中除了频率之外的输入信号的特性在计算中不被考虑，并且这是使用线性（S参数）模拟来完成的。
增益是不同的，因为它可以使用谐波平衡和线性模拟进行测量。
对于线性模拟，增益为dB（S21），这可以作为频率的函数而改变，但是是独立的信号幅度。
对于谐波平衡，增益可以测量为Pout / Pin，但可以定义为不同的频率（谐波），也可以表示为输入信号幅度的函数，这显然是P1dB测量的一部分。
在谐波平衡仿真期间还可以使用非线性噪声功能，该功能执行与小信号线性仿真相同但在大信号条件下的一些相同的测量。
现在要注意的重要一点是，线性和非线性模型都可以用于线性和谐波平衡模拟。
但它们只会在模型允许的范围内工作。
因此，例如使用线性模拟，可以使用线性s参数模型或非线性模型（只要应用所需的偏差）。
如果模型被正确提取和设置，两者都应该有希望模拟并给出类似的结果。
在这种情况下，非线性模型仅在线性模式下运行，因此它不会表现出任何增益压缩或产生任何谐波音调。
类似地，对于谐波平衡模拟，可以使用线性s参数模型或非线性模型（只要应用所需的偏差）。
在这种情况下，虽然不同类型的模型不会模拟并给出相同的结果。
在这种情况下，线性模型将仅在线性小信号模式下工作，并且永远不会表现出任何增益压缩或产生任何谐波音调。
如果这种类型的模型是电路中使用的唯一设备模型，那么谐波平衡将不会模拟任何功率相关行为（P1dB），频谱音生成或互调（IIP3或OIP3）。



     以下为原文

  You should really not consider this situation a question of what model can do what sort of measurement. It is completely based on the simulator you are using.

For example IIP3, OIP3 and P1dB compression are large signal measurements, the response of the circuit depends on the characteristic of the input signal(s), i.e. amplitude, DC offset etc., and these can be done using Harmonic Balance simulation.

Noise Figure and stability are typically small signal measurements, where the characteristics of the input signal(s), except frequency, are not considered in the calculations, and this is done using Linear (S-Parameter) simulation.

Gain is different as it can be measured using both Harmonic Balance and Linear simulation. For Linear simulation the gain is dB(S21) and this can change as a function of frequencey but is independant signal amplitude. For Harmonic Balance the gain can be measured as Pout/Pin but can be defined at different frequencies (harmonics) and can also be expressed as a function of input signal amplitude and this is obviously part of the P1dB measurement.

There is also a Non-Linear Noise capability available during Harmonic Balance simulation which performs some of the same niose measurements as the small signal Linear simulations but under large signal conditions.

The important thing to note now is that both linear and non-linear models can be used both Linear and Harmonical Balance simulations. They will though only work to the extent that the model allows in each case.

So for example with Linear simulations it is possible to use both a linear s-parameter model or a non-linear model (as long as the required bias is applied). Both should hopefully simulate and give similar results if the model was extracted and set up correctly. The non-linear model in this case will operate only in a linear mode so it will not exhibit any gain compression or generate any harmonic tones.

Similarly for Harmonic Balance simulations it is possible to use both a linear s-parameter model or a non-linear model (as long as the required bias is applied). In this case though the different types of model will not simulate and give the same results. In this case the linear model will only ever work in a linear small signal mode and will never exhibit any gain compression or generate any harmonic tones. If this type of model is the only style of device model used in the circuit then Harmonic Balance will not simulate any power dependant behavior (P1dB), spectral tone generation or intermodulation (IIP3 or OIP3).

这样没有+'错误'+。
使用线性模型将模拟结果与使用等效非线性模型的模拟结果进行比较可能永远不会产生完全相似的结果。
它们应该很接近，但除非为一个特定的操作点提取模型，否则两组模拟数据很少会给出完全匹配。
它们的接近程度取决于模型提取的质量。
通常从一组测量的s参数数据文件和偏差数据中提取非线性模型。
对于此设备，有12个s参数数据文件可用。
进行提取并进行优化，以在所需的整个偏置条件下提供最佳匹配。
仅关注一个偏置点并期望在该点处精确匹配是不现实的。
*注*：在您的设计中，在偏置电路中使用串联电阻会浪费功率。
应移除电阻器R3和R4或将其设置为0欧姆。
然后，您应该能够调整R1（更小？）以获得所需的Ids，并将Vdc直接设置为所需的3.0V。
使用DC模拟来验证这一点。
对于您的其他问题：* 1）*一旦设计中包含布局寄生效应，无论使用何种型号，都可能会改变任何电路的性能。
这种寄生在设备外部，因此完全独立于模型。
它不会修改性能以更好地匹配一种模式或另一种模式。
它会影响两者。
* 2）*除了大信号非线性测量外，您不需要做任何特定方法。
您可以使用最适合应用程序的任何内容。
因此，增益可以作为线性模拟或非线性模拟的一部分进行测量。
如果使用线性模拟进行测量，则可以使用线性模型或非线性模型。
如果使用非线性模拟进行测量，则s参数模型将无法正常工作，因此您需要使用非线性模型。
对于稳定性和噪声系数这些通常使用线性模拟方法完成，因为它是一个小信号测量，为此您可以自由使用线性或非线性模型。
IIP3，OIP3和P1dB压缩点作为非线性模拟的一部分进行测量，因此对于这些，您必须使用非线性模型。
* 3）*无论您使用线性模型还是非线性模型，都只与模拟有关。
在为设计创建布局时，这将使用物理器件封装的覆盖区来表示晶体管，并且与仿真模型无关。
在布局中，您需要包含所有必要的电路，以使晶体管偏置工作。
因此，为了准确性，用于仿真的原理图应表示与布局，相同组件和相同连接相同的设计。
因此，当使用S参数模型执行仿真时，您仍应包括所有组件和连接，这只是偏置电压无关紧要。
您可以将电压源设置为0V或1kV。
它不会产生任何影响，或者可以用S参数仿真的接地（短路）连接代替直流电源。
* 4）*虽然在所有情况下创建集总元件的分布式等效物可能并不重要，但在创建高频电路设计时始终是一个选项。
无论何时完成，尽管最好包括在设计中，如果您希望使用S参数或谐波平衡模拟器模拟设计，所有可能的寄生和不连续模型，包括弯曲，三通，十字架，台阶等。如果您是
使用EM仿真来模拟电路中的这些分布式结构然后这不是必需的，因为EM仿真将自动计算这种寄生效应。



     以下为原文

  There is no +'mistake'+ as such. Comparing simulation results using a linear model to any using the equivalent non-linear model will likely never yield exactly similar results. They should be close but unless the model is extracted for one specific operating point comparing the two sets of simulation data will rarely give an exact match. How close they get will depend on the quality of the model extraction. The non-linear model is typically extracted from a set of measured s-parameter data files and bias data. For this device there are 12 s-parameter data files available. The extraction is them performed and optimized to give the best possible match over the whole set of bias conditions required. Focusing on only one bias point and expecting an exact match at that point is not realistic.

*Note*: In your design using series resistors in the bias circuit is wasteful of power. The resistors R3 and R4 should be removed or set to 0 ohms. You should then be able to adjust R1 (smaller?) to get the required Ids with Vdc set to the desired 3.0V directly. Use a DC simulation to verify this.

For your other questions:

*1)* Once layout parasitics are included in a design this will likely modify the performance of any circuit regardless of the model used. Such parasitcs are external to the device so totally independant of the model. It will not modify the performance to better match one style of model or the other. It will affect both.

*2)* You do not need to do any particular method except for the large signal non-linear measurements. You can use whatever is best for the application.

So Gain can be measured as part of a linear simulation or a non-linear simulation. If you measure this with a linear simulation you can use either the linear or the non-linear model. If you measure this with a non-linear simulation the s-parameter model will not work correctly so you need to use the non-linear model.

For Stability and Noise Figure these are usually done using linear simulation methods as it is a small signal measurement and for this you are free to use either linear or non-linear models.

IIP3, OIP3 and P1dB Compression Point are measured as part of a non-linear simulation so for these you must be using a non-linear model.

*3)* Whether you use a linear or non-linear model for the device is relevant for simulation only. When you create the layout for the design this will use a footprint of the physical device package to represent the transistor and that is independant of the simulation model. In the layout you need to include all the necessary circuitry to bias the transistor for it to work. So for accuracy your schematic used for simulation should represent the same design as the layout, same components and same connectivity. So when performing simulation with S-Parameter model you should still include all the components and connections it is just that the bias voltage is irrelevant. You could set the voltage source to 0V or 1kV. It will not make a difference, or the DC source could be replaced by a ground (short circuit) connection for S-Parameter simulation.

*4)* Although it may not be essential in all cases creating a distributed equivalent for a lumped element prototype design is always an option when creating a high frequency circuit design. Whenever this is done though it is always best to include in the design, if you wish to simulate the design with S-Parameter or Harmonic Balance simulators, all possible parasitic and discontinuity models including bends, tees, crosses, steps etc. If you are going to simulate these distributed structure in the circuit using EM simulation then this is not necessary as the EM simulation will calculate such parasitics automatically.

sdgrant先生，我有太多的困惑和怀疑。
现在一切都从你的答案中解脱出来，我非常感谢你并感激你。
你帮了我很多工作。
先生，现在我想将IIP3，OIP3，P1 dB压缩绘制到我之前公布的非线性设计原理图中。
先生，我需要ADS 2009的PDF格式帮助文件，可能只有一个简单的例子，就这个例子而言，他们可能已经绘制了IIP3，OIP3,1dB压缩点，功耗计算。
您是否知道上述要点的ADS2009 PDF格式帮助文件的链接？
如果你给我看链接，对初学者来说这对我很有帮助。



     以下为原文

  sdgrant Sir,
                         I had so many confusions and doubts. Now everything cleared from your answers, I am really thankful and grateful to you. You helped me lot for my work. Sir, now I want to draw IIP3,OIP3, P1 dB compression to my previous posted schematic of nonlinear design. Sir I need PDF  format help file of ADS 2009, which may be having one simple example , with respect to that example, they might have drawn IIP3, OIP3,1dB compression point, power dissipation calculation. Do you know the link for the PDF format help file
of ADS2009 for above said points. If you show me link, it will be very much helpful for me like beginners.

ADS随附您需要的一切。
只需打开一个新原理图并选择“插入”>“模板...”，然后选择并放置相应的模板。
对于P1dB压缩，请使用HB1ToneSwptPwr模板。
将LNA放入原理图（带有必要的电压源）并设置RFfreq的值，并在扫描计划中设置输入源功率参数。
结果数据显示包括预先配置的表格和图表，显示功率增益，输出频谱和谐波功率电平。
对于IIP3和OIP3，请使用HB2ToneSwptPwr模板。
将LNA放入原理图（带有必要的电压源）并设置RFfreq，fspacing的值，并在Sweep Plan中设置输入源功率参数。
结果数据显示包括预先配置的表格和图表，显示低侧和高侧音调的输入TOI（IIP3）和输出TOI（OIP3）。
也是五阶拦截点。



     以下为原文

  ADS ships with everything you need. Just open a new schematic and select Insert > Template... then select and place the appropriate template.

For P1dB compression use the HB1ToneSwptPwr template. Drop your LNA into the schematic (with necessary voltage sources) and set values for RFfreq and in the Sweep Plan set the input source power parameters. The resulting data display includes pre-configured tables and plots that display Power Gain, Output Spectrum and Harmonic Power levels. 

For IIP3 and OIP3 use the HB2ToneSwptPwr template. Drop your LNA into the schematic (with necessary voltage sources) and set values for RFfreq, fspacing and in the Sweep Plan set the input source power parameters. The resulting data display includes pre-configured tables and plots that display Input TOI (IIP3) and Output TOI (OIP3) for both low side and high side tones. Also fifth order intercept points.

sdgrant先生，我按照你的说法尝试过，他们很有效率。
最后如何找到LNA的群延迟变化，我需要使用哪个模板来绘制群延迟变化。我尝试使用S_ParamsLargeSignal模板，它给出了错误。我需要使用哪个模板来测量群延迟变化和品质因数
（FOM）。



     以下为原文

  sdgrant Sir,
                     I tried as you said, magnificiently they are working. Last how to find the group delay variation of the LNA , which template I need to use to plot group delay variation.I tried using S_ParamsLargeSignal template, it was giving error.which template I need to use for measuring group delay variation and figure of merit(FOM).

sdgrant先生，我想找出1到2 GHz的带宽，ADS2009中有任何选项可以找出带宽。
上一篇文章你告诉dev_lin_phase（）测量（找出功绩图），它在ADS中可用。
我没有在帖子中找到前面的内容，你告诉你的优点，你已经显示出来。要找出BW，最大值下降3dB，后来我们标记fH和fL，然后减去fH-fL = BW这是正常的
找到BW的方法
ADS2009中是否有任何选项可直接查找B.W.
你能告诉我先生和dev_lin_phase，它在哪里。



     以下为原文

  sdgrant Sir,
                      I want to find out Band width from 1 to 2 GHz,any option is available in ADS2009 to find out Band Width. Previous post you told dev_lin_phase() measurement(to finding out Figure of Merit), where it is available in ADS . I didn't get previous in the post,what you told about Figure of Merit, where you have shown.To find out B.W, take maximum down 3dB , later we mark fH and fL ,and subtract fH-fL=B.W.This is normal way of finding B.W. Is there any option in ADS2009 finding directly  B.W. Can you tell me sir and also dev_lin_phase, where it is there exactly.

在在线帮助中，搜索关键字“bandwidth_func（）”



     以下为原文

  In the online help, search for keyword "bandwidth_func()"

sdgrant先生，我得到了关于品质因数和群体延迟变化的结果，你帮助我完成了我工作的每一步，谢谢。
现在我有线性和非线性器件模型的集总元件模型，使用不同的参数测量，如增益，噪声系数，稳定性，iip3，oip3，群延迟变化，带宽，功耗，品质因数等...
...我想制作线性和非线性器件模型，使用网络分析仪或频谱分析仪测量实际值，然后我必须比较测量值和模拟值。
我的问题是，我需要为线性和非线性器件模型创建布局，以制作两种模型。
我不能直接去没有布局的集总元素模型。
所以我是初学者，我必须如何创建布局，我应该用分布式元件替换像电感器这样的集总元件，在我为集总元件模型制作之前我必须做些什么。
请指导我，这对我的工作非常有帮助。有任何PDF格式帮助创建布局，你能告诉我链接。



     以下为原文

  sdgrant Sir,
              I got the results for both figure of merit and group delay variation, you helped me lot each and every step of my work, thank you. Now I have the lumped elements models of both linear and nonlinear device models, have measured using different parameters like, gain, noise figure, stability, iip3, oip3, group delay variation, band width,power dissipation, figure of merit etc...... I want to go for fabrication of the linear and nonlinear device models to measure practical values using network analyzer or spectrum analyzer, then I have to compare both measured and simulated values. What is my question is, I need to create layout for both linear and nonlinear device model for fabrication of both models. I can't go directly lumped element models of both without layout. So I am beginner, how I have to create the layout , shall I replace the lumped elements like inductor with distributed elements, what I have to do before going to fabrication for my lumped element models. Please guide me, it would be very much  helpful for my work.Is there any PDF format help for creating layout, can you show me link.

你说你现在想要“为线性和非线性器件模型创建布局以制造两种模型+”，但实际上这些只是对同一个封装器件进行建模的两种不同方法。
一个是直接测量的s参数数据文件，即您使用的线性模型。
另一个是从测量的DC偏差和s参数数据导出的数学模型，在这种情况下是非线性模型。
无论是否使用模拟设备的线性或非线性模型表示，您为此电路创建的布局都应相同。
外部信号源（DC和AC / RF）可能是不同的，但电路拓扑和配置应该相同。
从这一点开始如何进行布局完全是您必须做出的设计选择。
ADS当然可以是您可以用来实现设计的工具，但您必须根据您要使用的制造技术的限制自己做出必要的设计选择。
没有明确的分步流程可以为您做出这样的设计决策。



     以下为原文

  You say that you now want to "+create layout for both linear and nonlinear device model for fabrication of both models+" but really these are just two different methods of modeling the same packaged device. One is a set of direct measured s-parameter data files, the linear model you used. The other is a mathematical model derived derived from measured DC bias and s-parameter data, the nonlinear model in this case. The layout you create for this circuit should be the same whether you use the linear or nonlinear model representation for the device for simulation. The external signal sources, both DC and AC/RF, may be dirfferent but the circuit topology and configuration should be the same.

How you proceed to layout from this point is entirely a design choice that you have to make. ADS certainly can be the tool that you can use to implement your design but you have to make the necessary design choices yourself depending on the constraints of the manufacturing technology you are to use. There is no definitive step-by-step process that will make such design decisions for you.

尽管曲线追踪器可以完成任务，但它似乎是一种不必要的复杂方式。
曲面跟踪器通常用于表征器件，在这种情况下，FET本身可以在设计电路之前确定器件的最佳工作点。
它在整个DC工作点范围内进行扫描DC分析。
当您想要表征完成的电路时，您只需要模拟电路使用的单个DC工作点，因此不需要扫描测量。
只需使用固定直流电源进行简单的分析即可。
在侧面点，您在原理图中显示的扫描电压设置配置为从-2V到0V的Vgs扫描。
负电压。
那是对的吗？
您之前包含的原理图具有正Vgs DC源。



     以下为原文

  Although the curve tracer would do the task it seems an unnecessarily complicated way of doing it. The curver tracers are usually used to characterize the device, a FET in this case, on its own to determine the optimum operating point for the device prior to designing the circuit. It does a swept DC analysis over a whole range of DC operating points. When you want to characterize a completed circuit you only need to simulate the single DC operating point that the circuit uses so swept measurements are not needed. Just do a simple analysis on its own with fixed DC sources.

On a side point the sweep voltage setup you show in your schematic is configured for a Vgs sweep from -2V to 0V. Negative voltages. Is that correct? The schematic you included earlier had a positive Vgs DC source.

由于两个原因，这是不正确的。
您不需要使用曲线跟踪器进行任何扫描DC模拟。
这是615（15x41）扫描点DC模拟。
您只需要在LNA所需的DC工作点进行一次模拟。
与先前用于非线性模拟的相同的示意图应当正确地工作。
在此模拟中，您似乎使用3V，60mA s参数数据文件作为FET的模型。
这对DC模拟不起作用。
s参数模型旨在用于s参数/线性仿真或非线性仿真，其中它是像滤波器一样的无源电路。
对于DC模拟，它只能用作电阻网络。
Vgs的变化不会改变晶体管中的Ids。
您需要使用设备的非线性模型进行DC分析。



     以下为原文

  It is not correct for two reasons.

You do not need to do any swept DC simulations using the curve tracer. This is doing 615 (15x41) swept point DC simulations. You only need one simulation at the required DC operating point of the LNA. The same schematic as was used for the nonlinear simulation previously should work correctly.

It seems you are using the 3V, 60mA s-parameter data file as the model for the FET in this simulation. That will not work correctly for DC simulations. The s-parameter model is intended for use in s-parameter/linear simulations or in nonlinear simulation where it is a passive circuit like a filter. For DC simulations it will only work as a resistive network. Changes in Vgs will not change Ids like it should in a transistor. You need to use the nonlinear model for the device to do DC analysis.

sdgrant先生，由于服务器问题，我发布了相同的5个帖子。
相同的帖子已经出现了5次。
对不起。



     以下为原文

  sdgrant Sir,
                    I have posted same 5 postings due to server problem. Same posting has appeared for 5 times . I am sorry.

这就是我要做的。
1.切勿使用线性s参数模型进行任何测量。
您可能会得到答案，但这些模型从未用于DC模拟。
仅使用非线性模型。
2.停止使用Curve Tracer仪器。
只需使用常规直流电压源进行直接直流模拟，您必须对电路进行偏置并添加电流探头。
（实际上只是考虑一下如果你使用的是Curve Tracer并且你仍然在你的电路中有DC源，你没有显示它是如何连接的，那么这就是问题的原因.Curve Tracer有自己的内置
-in电压源。）3。当前面讨论的电阻器时，我建议你应该只有2个电阻器。
漏极连接（R4）中的电阻应为零，栅极连接（R3）中的串联电阻应为零，只有两个分流电阻（R1和R2）。



     以下为原文

  Here's what I would do.

1. Never do any measurements using the linear s-parameter model. You may get answers but these model are never intended for DC simulations. Use only the nonlinear model.
2. Stop using the Curve Tracer instrument. Just do a straight DC simulation with the regular DC voltage sources that you already have to bias the circuit and add current probes. (Actually just thinking about it if you are using the Curve Tracer AND you still have the DC source in you circuit, you didn't show how it was connected, then that is the cause of the problem. The Curve Tracer has its own built-in voltage sources.)
3. When the resistors where discussed earlier I recommended that you should have only 2 resistors. There should be zero resistance in the Drain connection (R4) and also be zero series resistance in the gate connection (R3), only the two shunt resistors (R1 and R2).