OPA683: OPA683 versus OPA684 input offset voltage in TINA models

Below is the spice circuit:

Hi, 

Can you tell me what is connected on the other side of your gain resistor? Is it just grounded or do you have another resistor connected. The input bias current flowing through the resistor will also add offset that is independent of the input voltage offset of the amplifier. 

Regards, 

If I run the two reference designs and look at the inverting node voltage for 0V V+ input, the OPA684 is about 270uV and the OPA683 is about 170uV. Likely you are getting into some Ib- errors. 

The input of R2 is the output of a trans impedance amp.

The input bias for the 683 is +/- 3uA (typical) and for the 684 is +/- 5uA (typical), so I don't think this is the factor here.

I this just errors / differences in the spice models?

Thanks

Hey Chris, to resolve, it would be helpful you would attach your TINA files. 

I have tried running both 684 and 683 with a gain of 1 with a square wave input simulating my downstream circuit (see attached TINA model).

The OPA683 results in a larger output offset than the OPA684 even though both have similar offset voltages (+/- 1.5 mV) and the OPA684 has a larger inverting input bias (+/- 5 uA versus +/- 3 uA)

684_or_ 683_only.TSC

Well Chris, you cannot float the disable pin, must tie to +Vcc, Doing that and simplifying your setup a bit, gives these DC errors (I also set you input to have a 0V DC) OPA683 first, The bias current seems a little high here and the offset seems low - but these just what this transistor level model is producing. 

Then the OPA684 in the same ckt. bias current seems right, offset seems low. 

So these differences are very likely just model Spice model imperfections even though the OPA683 and OPA684 show very similar spec in the data sheets?

BTW if I change the square wave input to a simple -1V DC input (and have Disable connected to +5VDC),

The OPA684 shows a -245uV offset (on the inverting input) However

The OPA683 shows a +2.21mV offset (on the inverting input) 

This seems very odd

You have something else going on in your setups, if I add a -1V DC to the input signal, I get 162uV on the V- node

Thanks for your help Michael.

The problem seems to be in TI TINA spice model.

I have been using the OPA683 under the Spice Macros tab of Tina SPICE (which yields the 2.21mv offset)
when I swap the spice macro OPA683 with the OPA683 from the reference design, I get an offset of 162uV.
when I delete the ref design OPA683 and try to replace it with the Spice Macro OPAMP OPA683,  and then run DC Analysis, I get the following error:

"Missing syntax element.Line #1.(OPA683).

This suggests the spice model for the OPA683 under the SPICE Macros OP AMP menu is incorrect or has issues!?!?

Now not sure what to trust on any of my previous simulations.

Hey Chris, 

If you right click on the symbol, a menu will open where at the bottom is an enter macro to see the netlisting. To get out of that in the upper left hand is a close icon, 

Anyway, I don't think DesignSoft updates their library very much (if at all) the TINA library model is 2002 original - 

The product landing page model is a 2011 update, I always suggest to use the latest on the product folder - those get updated kind of randomly. This was using a 2008 revised datasheet. 

Actually what I think you got into was that DesignSoft does not update their libraries much. While their library is usefull, I have decided to always check if there is a newer one on the product folder. Normally, models are not updated unless they are getting better.