i try to use ad8338 spice model, but it doesn't work, there is an error in line 72. Any suggestion how to solve it?

i try to use ad8338 spice model, but it doesn't work, there is an error in line 72. Any suggestion how to solve it?

ruggiLucio,

Over the years, different companies have added supersets to the basic spice commands.

The "Limit" function is quite useful, but as you noted, TINA doesn't like it. We do try to

write spice models with only the basic Spice 2g6 syntax, but the limit function is quite

useful and most simulators now handle it.

Harry

**ruggiLucio,**Might be a bit late..but

**I also have been through this. There are different Spice syntax types e.g. Berkeley SPICE3 which some simulators can't handle. There's nothing wrong with Tina-Ti. It's great.**The support from manufacturers of the IC's is the problem not being able to help with these models. One model can work with one simulator but not another!! Frustrating.

2 lines have to be re-written in the AD8338 model for Tina-Ti.

Was

- BSLEW VSLEW 0 I=(-1)*LIMIT((V(VGAINOUT)-V(VSLEW)),0.002,-0.002)

Now

- GSLEW VSLEW 0 VALUE ={(-1)*LIMIT((V(VGAINOUT)-V(VSLEW)),0.002,-0.002)}

Was

- BCLAMP VLIMIT 0 V=LIMIT(V(VPRE), 1.55, -1.55)

Now

- ECLAMP VLIMIT 0 VALUE {LIMIT(V(VPRE), 1.55, -1.55)}

This is the sort of answer we want from manufacturers!!!

ruggiLucio,

Over the years, different companies have added supersets to the basic spice commands.

The "Limit" function is quite useful, but as you noted, TINA doesn't like it. We do try to

write spice models with only the basic Spice 2g6 syntax, but the limit function is quite

useful and most simulators now handle it.

Harry