CALCULATOR DNL/ INL DAC

I made a waveform for testing

The result of the dnl function is as follows
Which is the X-axis and the Y-axis are in terms of voltage

The result of the dnl function in mathlab is as follows
Which is the X-axis in terms of time and the Y-axis are in terms of voltage

As is clear from the signal of the value (0v to 1.8v) after that (1.8v to 0v) after that (0 to 3.2)

And because one axis is in terms of voltage and the other is time, the waveform is not the same.

you can't use the YvsY() function
i use dc signal 0v as the time axis as a waveform (/net011)
when i plot two out put in simulation Draws them in the subwindows form

I can use YvsY for (/net11) and (/net05)  Because both of the in same windows and choose select trace 

i can not plot inl and (/net11) in same window that YvsY

What should I do to solve the problem?

In your opinion, it is not better to write a program VHDL or verilog

Dear mirtaji65,

mirtaji65 said:

What should I do to solve the problem?

I hope the following solves your latest problem. I have included the specific steps I followed and the resulting plots of INL versus voltage and the new plot of INL versus Time.

Shawn

1. Create time values:

value(v("/vout" ?result "tran") 0.5e-06  ?period 1e-06 ?xName "time"  )

Place in Calculator Table (Tools->Table)

2. Create inl values:

value(inl(v("/vout" ?result "tran") 1e-06  ?mode "auto"  ?crossType "rising" ?delay 0.5e-06 ?units "abs" ?nbsamples nil) 0.5e-06 ?period 1e-06 ?xName "time")

Append to table (See below for comma-separated variable file I created)

3. Save table as a comma-separated variable file with <filename> (i.e. nl_xval_inl.csv)

3.Create new waveform:

getAsciiWave("Full path to saved file inl_xval_inl.csv"> 1 4 ?xskip 1 ?yskip 1 ?formatFloat nil ?xName "Time" ?xUnits "sec" ?yName "inl" ?yUnits "LSB" )

4. Plot new waveform

5. Enjoy!

Example "inl_xval_inl.csv"

time (s),xval(value(v("/vout" ?result "tran") 0.5e-06  ?period 1e-06 ?xName "time"  )) (s),V (V),inl
500.00000E-9,500.00000E-9,24.961888E-3,0.0000000
1.5000000E-6,1.5000000E-6,72.934183E-3,-37.478530E-3
2.5000000E-6,2.5000000E-6,123.74225E-3,-18.059857E-3
3.5000000E-6,3.5000000E-6,175.35193E-3,17.442537E-3
4.5000000E-6,4.5000000E-6,223.30014E-3,-20.519130E-3
5.5000000E-6,5.5000000E-6,276.42237E-3,45.331194E-3
6.5000000E-6,6.5000000E-6,323.72824E-3,-5.5186424E-3
7.5000000E-6,7.5000000E-6,374.44416E-3,12.051288E-3
8.5000000E-6,8.5000000E-6,425.94798E-3,45.429609E-3
9.5000000E-6,9.5000000E-6,474.45422E-3,18.664130E-3
10.500000E-6,10.500000E-6,524.10157E-3,14.794140E-3
11.500000E-6,11.500000E-6,576.87473E-3,73.640760E-3
12.500000E-6,12.500000E-6,622.86814E-3,-3.5422922E-3
13.500000E-6,13.500000E-6,675.23440E-3,47.140060E-3
14.500000E-6,14.500000E-6,722.63109E-3,-1.8875072E-3
15.500000E-6,15.500000E-6,772.56539E-3,-555.11151E-18

sml 1/4/2021

Dear Shawnlogan

Your solution for converting X-axis from voltage to time works exactly.

But why do I have to sample the waveform by use <<value function>>  when i want to use INL and DNL function ,why delay of INL function doesn't work itself,

Is this a software bug?

ver virtuoso :6.17.77

This method is not suitable if I want to use the analysis parameter

But your method of  converting X-axis from voltage to time  was great

thanks my friend

Dear mirtaji65,

> Your solution for converting X-axis from voltage to time works exactly.

Great! Thank you for letting us know!

mirtaji65 said:

But why do I have to sample the waveform by use <<value function>>  when i want to use INL and DNL function ,why delay of INL function doesn't work itself,

Is this a software bug?

First, I do not work for Cadence and hence cannot really respond to your comment about the behavior of INL. However, the INL function, as it is documented, does not provide the x-axis as a function of time (which is what I assume you want). Hence, the "workaround" using the value() function.

mirtaji65 said:

This method is not suitable if I want to use the analysis parameter

Sorry, I don't understand exactly what you mean by this comment! You can use this methodology in an Explorer/Assembler expression through the use of an ocean script. This is documented at URL:

https://support.cadence.com/apex/ArticleAttachmentPortal?id=a1Od0000000nXTvEAM&pageName=ArticleContent

and

https://support.cadence.com/apex/ArticleAttachmentPortal?id=a1Od0000000nXS2EAM&pageName=ArticleContent

Hence, you may define the steps in an ocean script and add the ocean script as an Explorer/Assembler output.

I hope this helps mirtaji65,

Shawn