AC Analysis in Advanced Design Environment (ADE)

Authors: Jihoon Jeong, Justin Cartwright, Dr. Dong S. Ha

This section will guide you to run AC analysis and utilize Calculator in ADE.

1. To start simulation, choose Tools->Analog Environment from the top menu in Schematic Editing window, Analog Design Environment (ADE) will appear. Click on Setup-> Simulator/Directory/Host…, choose spectre as the "Simulator" and click OK. Then select Variable->Copy from cellview, you will see all the variables defined in the schematic show up in "Design Variables section". Double click each variable and set its value as you wish. (Fig. 7) Here are my values.

Vac = 100 m, Vfreq = 500 M, Vdd = 1.8, Vdc = 1, Vamp = 100 m, R = 1K, N_finger = 10, L = 0, C = 10 f Note that we will give L value of 0, so there is no bandwidth extension at this point.

Figure 7. Assign design variables in ADE

2. Next select Analysis->Choose… or click on the Choose Analyses… button on the right toolbar. Choosing Analyses window will appear. This is where you have options to run many different types of analysis. Choose tran from "Analysis" and give a simulation time. (Fig. 8) Check moderate from "Accuracy Defaults" and hit Apply.

Figure 8. Choose Transient Analysis

3. To run AC analysis, choose ac from "Analysis" and Frequency from "Sweep Variable". Specify Sweep Range and Type. (Fig. 9) Hit OK.

Figure 9. Choose AC analysis and specify options

4. Before you start the simulation, let's add outputs to be plotted. Click Outputs-> To Be Plotted->Select On Schematic from the top-menu (Fig. 10) and click each node interested in Schematic Editing window. The node name will show up in Output section.

Figure 10. Add outputs from schematic

5. Make sure you hit "Check and Save" button from the left toolbar in Schematic Editing window and run simulation by hitting "green" traffic signal on the right toolbar in ADE window. (Fig. 11)

Figure 11. "Check and Save" and Run

6. You will be able to see a run log file and output graphs. The left graph shows the transient response and right graph plots the ac response of in/output signals. (Fig. 12)

Figure 12. Transient and AC response plots

7. Let's calculate a voltage gain to finally measure 3 dB bandwidth while sweeping L values. Click Outputs -> Setup from the top menu in ADE. The Setting Outputs window will pop up. (Fig. 13) Name your output defined (Gv) and click "open" button next to the Calculator.

Figure 13. Setting Outputs Window

8. The Calculator window will show up. (Fig. 14) Choose ac from "Selection choices" and click radio button for vf. (We are going to measure AC voltage)

Figure 14. Open Calculator and select ac

9. We will now measure a node voltage on the schematic. Click the Vout node in the schematic, VF("/Vout") appears in your Calculator box (Fig. 15). If you want to calculate dB20 (because it is a voltage gain not power gain), click dB20 in the filter box.

Figure 15. Specify measuring point and filter

10. Repeat same method to calculate Vin in dB20 scale and subtract it from Vout in dB20. dB20(VF("/Vout"))-dB20(VF("/Vin")) will appear in your Calculator box. Go back to Setting outputs window, click Get Expression from Calculator. The defined expression will show up in Expression box. (Fig. 16) Hit OK.

Figure 16. Get Expression from Calculator

11. Three graphs will be plotted if you run your simulation again. (Fig. 17)

Figure 17. Three graphs plotted

12. According to the Table 1. in the text book below, the maximum bandwidth can be obtained when m ~ 1.41. Let's calculate some inductor values before sweeping L values in the simulation.

We have used R = 1 K and C = 10 fF in the circuit. The L value for the maximum bandwidth will be calculated around 7.1 nH and 3.226 nH for the best group delay.

13. Let's sweep the L values. Click Tools->Parametric Analysis… from the top menu in ADE. (Fig. 18)

Figure 18. Launch Parametric Analysis window

14. Parametric Analysis window will pop up. You can make several sweeps for your simulation. We will sweep only one variable, L, at this point. Type L in "Variable Name" and Specify "Range Type" and "Step Control" in Sweep 1 section. Start analysis by clicking Analysis->Start from the top-menu in Parametric Analysis window. After 9 runs sweeping L values from 0 to 8 nH with 1 nH step, we will get 9 plots. (Fig. 19)

Figure 19. Start Sweep Analysis

15. Let's zoom in frequency between 1 GHz and 10 GHz by clicking zoom-in button on the top-menu. (Fig. 20)

Figure 20. Zoom in x axis

16. To place Market, click Market->Place->Trace Marker, Vert Marker, and Horiz Marker. (Fig. 21)

A 3dB bandwidth without L is about 13.48 GHz, a 3dB bandwidth with L of 8 nH (maximum) is measured about 24.37 GHz. (Fig. 21) A normalized bandwidth is 24.37/13.48 ≈ 1.8. I'll leave calculations of normalized bandwidth values for other conditions.

Figure 21. Place markers to measure 3dB

If you have any question regarding on this tutorial, please feel free to contact me, Jihoon Jeong. (jihoon@vt.edu)

Previous