This installment of the TINA-TI series is based on your requests from the list in Part 1. In this post we’ll learn how to generate:
Time varying source:
In practice, standard waveforms (i.e. square wave, triangular wave, etc.) may not suffice for your simulation and you may need to generate a real-life excitation waveform, similar to what is in your system, to verify bench behavior or to predict performance before you build. For these situations TINA-TI offers the piecewise linear source which can create either transient or repetitive waveforms.
The key to creating the piecewise linear source is to first put the time (x-axis) and voltage, or current (y-axis), in table form (x, y) and then insert it in the TINA-TI source information dialog. TINA-TI does the rest (see Figure 1).
Figure 1: Entering source (VG or IG) information that defines the time-variable waveform
You can even make the waveform repetitive provided one full x-y cycle is defined (see Figure 2)!
Figure 2: Adding simple text commands make the waveform repetitive
As you can see, it is very easy to make a single pulse or a portion of a waveform.
What if the waveform is more complicated, or if you want to use an extensive list of x-y points for more accuracy? What if you like to define the waveform algebraically (using an expression)? Simple!
Generate the x-y table in a spreadsheet program (like Microsoft Excel or equivalent) and copy and paste into the TINA-TI Signal editor panel. Figure 3 is an example of a waveform computed using Excel for a fast exponential rise time and a slow exponential fall time.
Figure 3: Using Excel to compute waveform
Figure 4 shows the resulting repetitive waveform in TINA-TI.
Figure 4: Resulting waveform copied and pasted from Excel
Frequency varying source:
TINA-TI has the ability to generate and preform AC Analysis with any waveform / source that is described with a Laplace transform expression involving “s”. This can be powerful in many simulation applications such as filters, electro-mechanical response, Laplace transform magnitude / phase visualization and many others.
Say you are contemplating the characteristics and the order of a filter you need in front of a fully differential amplifier (FDA), such as the 2.8GHz LMH6554, to drive a GSPS analog to digital converter (ADC), like the 12bit 1.6GSPS ADC12J1600, and you’d like to find out the overall response. You know that you will get a “smoother” response from a Butterworth filter, but a Chebyshev filter is bound to have a sharper skirt. If you simulate the response using the filters’ Laplace transforms, and implement your FDA design, you can get the actual response at the ADC input, including any effects from interaction of stages with each other.
You may also include any parasitics in your analysis. Figure 5 is one such example where U1 and U2 TINA-TI macros respectively represent 4th order 100MHz low-pass Butterworth and Chebyshev filters, driving identical LMH6554 single ended to differential amplifiers. Simulated AC analysis shows the overall transfer function.
Figure 5: Example of AC analysis using frequency variable sources (U1, U2)
The two identical LMH6554 stages used in Figure 5 are so that the two filter type (simulated by U1 and U2) responses can easily be compared side by side and on the same plot. “C_load” included in these simulations is meant to represent any parasitic cap (albeit greatly exaggerated here for emphasis) between the filter output and the FDA input which could affect the response.
Figure 6 shows how one would go about editing the frequency dependent sources (U1, and U2) to tailor these to fit the frequency characteristics we have in mind.
Figure 6: Right click on U1 or U2 macro to enter macro in order to change its characteristics
I hope you enjoyed this installment of the TINA-TI series. I look forward to your comments and questions. The files I used for this post can be found at the very bottom of the blog.
Check out my previous posts in this series to learn more about how TINA-TI can help in your designs. And, for more info on choosing the right filter for your design, check out my colleagues post called “Filter for thought” or the Webench Filter Designer tool.
A colleague had the following questions about the Macro in Figure 5, which is opened in Figure 6.
I've responded below for other people's benefit:
1. What element does E1 and EX represent?
RESPONSE: Essentially, the macro consists of two VCVS (E type) inside; the 1st one (on the input side, EX) takes the differential input at X1 and X2 and creates a voltage at node 1 relative to ground (with gain of 1V/V). The 2nd VCVS (E1), takes the node 1 voltage and does the Laplace transform operation on it.
2. From my understanding E1 is an element connected from Out to GND with the Chebyshev transfer function…is this correct?
RESPONSE: Yes, the E1 output terminals are tied to OUT and ground and it operates the Laplace transform on the node 1 (relative to ground).
3. I do not understand what EX is doing. Could you please explain.
RESPONSE: EX takes the differential input (X1 – X2) and creates a ground referenced voltage (node 1) which then E1 operates on, as explained in #1 above.
All content and materials on this site are provided "as is". TI and its respective suppliers and providers of content make no representations about the suitability of these materials for any purpose and disclaim all warranties and conditions with regard to these materials, including but not limited to all implied warranties and conditions of merchantability, fitness for a particular purpose, title and non-infringement of any third party intellectual property right. No license, either express or implied, by estoppel or otherwise, is granted by TI. Use of the information on this site may require a license from a third party, or a license from TI.
TI is a global semiconductor design and manufacturing company. Innovate with 100,000+ analog ICs andembedded processors, along with software, tools and the industry’s largest sales/support staff.