Re: Solutions for Microchip Opamps ?? ( MCP6001, MCP601, MCP616 )

--- In LTspice@yahoogroups.com, "matthiasltspice"
<matthias.hoffmann@...> wrote:
>
> Hello,
> I've read several messages about the problem with these
> Microchip - Parts. Even the NTC - Test - Circuit in the
> files section ( with the mcp601 ) doesn't work on my
> ltspice.

Hello Matthias,
I have tried a lot in the past and finally gave up
at that time.

> At the moment i am examining some small circuits
> ( differential amplifiers, various current sources )
> with several different opamps, especially the temperature
> drift of these opamps.

The models don't really contain useful models for
temperature. The reason is very simple. It would require
to use the worst case bias current and temperature drift
in the subcircuit model. No company want make their parts
looking bad, if the competition only provides models with
much better looking typical behavior.

Don't give a cent on any .TEMP with opamp models.
It will be totally wasted time and wrong too.
It can also corrupt the whole model behavior.
If you want model temperature behavior, you have to add
that externally using voltage and current sources.

If you look into the subircuit, you will see resistors
with TC=1 and TC=2. This means the resistors using this TC
will become negative resistance at negative temperature.
That can be another source for convergence problems if
you use a temperature below the SPICE nominal value(27°C).

> The result is the comparison
> between simulation and my smd-circuits. If there is no
> solution i will try to model these with pspice student
> edition (...in identical schematics it has exactly
> [10e-9V] the same results like LTspice...very fine...
> thank you LT...) but this accepts not 2 of these
> opampmodels because of the node limitation. Has anybody
> found a solution for using these models in ltspice?

I tried now again and had success. See my procedure below.

> I'll put a small test-circuit (voltage follower and
> non inverting amplifier) and the microchip.lib
> (including mcp6001,mcp601,mcp616) in the temp folder.
> Excuse my english and thank you for reading!!!
>
> regards,
> matthias


The procedure is as following.

Control Panel -> SPICE -> Reset to default settings

1. Make a transient simulation and save the steady state
bias point of all nodes in a file.

2. Use the data of this file in the .AC and .TEMP simulation.

3.
The temperature simulation has required an additional clamp
circuit at the opamps' output to achieve convergence above
94 degree.

I have added much more help text into my example schematic.

Files > Temp > microchip_conv_solution.zip

Best regards,
Helmut
