TINA/Spice/LP324-N: Filter Designer Tool vs Tina-TI

I use google chrome ... but flash needs to be enabled.

Did you try to understand the results you get?

webench_design_3569784_41.tscHi,

The problem is not with Tina-TI. My issue is with this. Is the magnitude response from Filter Desginer Tool based on assumption that OPAMP is ideal or does Filter Designer Tool use LP324-N spice model that TI is not willing to share. I dont really mind if the LP324-N is not shared i just want to be sure that results are realistic. I am asking because in Tina-TI there is a LPV324, LMV324N, LM324 and if use those in Tina-TI the results are not even close to what Filter Designer Tool does.

So if someone from TI can tell me when i do export design in Filter Designer Tool and i get ideal opamp will be used, does that mean that also Filter Designer is using ideal opamp?

Thank you

Hello Mirza,

Unfortunately, because the tool is so new it has some limitations which we are aware of and working to resolve.

To answer your question, the tool uses an idealized op amp and not a spice model of a real part.  After the simulation, the tool determines which part would work based upon the part's specifications.  The TINA spice simulation should help you to verify the results of the webench tool using the part's actual model.

However, there is no model of the LP324-N, neither public nor private.  This brings up a shortcoming of the tool.  It does not have a complete listing of all the parts available.  The consequence of this is that it may suggest older parts, which are less likely to have TINA models...such as the LP324-N.

The good news is that the web bench tool will provide accurate results with the assumption of an idealized op amp.  So, the real issue here is to determine how much performance you need out of your part.

I would suggest you consider two key specifications when selecting an op amp:  bandwidth and slew rate.

If you need help determining the minimum bandwidth required, you can use our FilterPro 3.1 tool to help.  This tool works very similarly to the webench tool.  Once you've completed your design using this tool, it will give you the minimum gain bandwidth product required of the part.

To determine the minimum slew rate required, you need to determine the maximum output voltage amplitude at your highest frequency of interest.  Then use the full power bandwidth formula to determine the minimum slew rate needed from your part.  For more information on this and the formula, see the final slide in this Precision Labs slide deck.

This should give you enough information to select your op amp.  You can use our Product Selection Guide for Op Amps to quickly search our product portfolio for the part(s) that will work best for your filter.

Please let me know if you have any further questions.

Daniel

Hi Mirza,

here comes a TINA-TI file which works:

mirza1.TSC

Kai

Thank you for a very detailed answer. I understand now much more.

I am building something that is has power supply 0 to 3.3V. I see that even when i choose the opamp based on BWD, slew-rate and that it can work for 1.8-5 power supply, if i set power supply 3.3V the results in Tina-TI are not correct. Only after setting power to 5V i get something. Is this Tina-TI limitation or model limitation?

Mirza 

Hi Kai

Thank you for the sim. Now can i ask you to choose an opamp that you know works for low power supply form 1.8-5 (on positive supply), then tie all negative power supply pins to GND and all positive power supply pins to 3.3V and run the simulation again.

What do you get?

Like this, for instance:

mirza2.TSC

Kai

Hi Kai and Daniel

thank you very much for the support. 

I am attaching a design from filter designer tool. I set fc=60, BW=1 Att = -40dB and under design i set ideal values for resistors and capacitors. When i ask for export i am informed that an ideal OPAMP will be used. I run the simulation and i get nice results (which is nice). Even the filter tool sets Vcc=3.3V and Vee=0, so it is a single ended supply. I looked on TI web page for op amp with single ended supply and i found LMV612. When i insert in the design the LMV612 i do not get the results even close enough. 

Can you suggest or try to explain what is happening

Thank you

NotchFilter_FilterDesignerTool.TSC

Hi Mirza,

as Daniel mentioned, the web bench tool does not work properly right now, but makes mistakes. So, I would not trust it. TI should explain the user in detail which feature of the web bench tool is working and which is not.

Anyway, what is wrong with the schematic I gave you? Have you understood why a midsupply bias voltage is necessary, when the circuit is powered by a single supply voltage? Please go into my "mirza2" simulation and do some "DC Analysis" by using the tool "Calculate nodal voltages". Then you will see, how all the signal nodes are biased at midsupply. Also note the necessity of cap C5.

Kai

Hi Mirza,

sorry, sometimes I'm a bit impulsive... :-)

Please don't hesitate to ask me, if you have any question about the circuit.

Kai

Hi Mirza,

I have had a closer look at your last web bench tool simulation. One important point of critcism is, that the web bench tool gives you much too small feedback resistors: R3_S1 = R4_S1 = R3_S2 = R4_S2 = 30 Ohm is totally unrealistic! The consequence would be huge signal currents which the OPAmp cannot deliver at all. Probably the web bench tool has dictated a filter capacitance of 1µF and calculated from this the feedback resistances. In my "mirza2" simulation I have corrected this and have increased the feedback resistances and decreased the filter capacitance, so that the product of both and by this the corner frequency remains the same.

Another important issue is, that these kind of circuits react very sensitively to manufacturing tolerances of components. In the following simulation I have assumed realistic manufacturing tolerances of about 1% for some of the resistors and 5% for some of the filtering capacitors:

So, it's very important to use very precise resistors and filtering capacitors which should also show only very little long term drift and temperature drift. Polystyrene caps should be preferred, if possible providing 1% (< 5%) manufacturing tolerances. Additionally, it's a good idea to make some of the resistors trimmable. By this the influence of manufacturing tolerances can be furtherly reduced. In my simulation are these R5 and R11, for instance.

Kai