Question about HSpice & Spectre

[tedchen]

spectre diode model

My simulation is about radiation impact so there will be a hugh current
occurs at probably any node of my circuit. The voltage at the node
which got hit will rises of falls extremely fast, that's ok, that's what we
expected. What we didn't expected is that voltage rises above Vdd, say,
20V @ 2V circuit, or below ground. My opinion is, if the bulk-drain and
bulk-source diodes are counted, I think the rising or falling voltage will
stay within certain range.

I know both spice and spectre probably use something like voltage
controlled capacitor for those diode. However, those capacitance won't
keep the current and voltage within limited values.

So, my question is, how to make those simulator to simulate "real" diode?

 

[dumeHCM]

calcacm default

It doesn't matter. Use the simulator that the models of your devices are available

 

[tedchen]

spectre diode capacitance

It doesn't matter. Use the simulator that the models of your devices are available

I can use HSpice or Spectre, and I know simulator doesn't matter.

All I am asking is, how to make those two simulators to simulate
the circuit with diodes at each drains and sources.

In simulation, there are no diode at drains and sources, just some
capacitors. However, in real circuits, in real MOS transistors, there
are PN junctions, there are diodes. I heared that there is some
options or settings can let me set the simulator to simulate "diodes"
not "capacitors." I checked the HSpice manual, ACM option seems
will make my day, but it didn't.

 

[sunking]

You can add a diode in the schematic for simulation.

 

[tedchen]

You can add a diode in the schematic for simulation.

Yes, I know I can add diodes in the circuit, and that will be my last choice. The Hspice manual does indicate that MOS transistor model has two diodes: bulk-source, and bulk-drain. There are some equations for MOS diode. However, based on simulation results, I don't think that the simulation matrix counts those diodes simply because the diodes should clamp the voltages but it didn't happen.

As I said, adding the diodes to the circuits will be my last choice. I got more than 50 transistor in my circuit and I will have to add more than 100 diodes to each drains and sources. Furthremore, I have to calculate the PD, PS, AD, AS to define the diodes, I suppose.

I think the manual mentions MOS diode for a reason and I just have no idea how to force the simulator to take those diodes into consideration. I tried the ACM option, didn't work.

Does anyone know how to do this?

 

[tedchen]

Finally, I got it working.

I think I'd better share this with you guys in case someone got similar problem. I am using TSMC 0.24um and TSMC 0.18um. I am not sure is this solution will fit other process.

The MOSIS test data doesn't include the ACM. All you have to do is add ACM=0~3 in the model then simulate.

If you got the official spice model released by TSMC from somewhere else, it got ACM and CALCACM inside the model. The default values is 1 for CALCACM and 12 for ACM. CALCACM=1 and ACM=12 means using the MOSFET diode with Berkeley diode calculations, which sucks, in my opinion. Change the CALCACM to 0 and ACM to 0~3, depends on your requirements, then it should work.

Ted

 

[micel99]

That's great! Ted, thanks for sharing this out. If we didn't know this, where could we find definition of CALCACM, ACM levels?

 

[alenhan]

the model of Hspice and Spectre have differenc format, you should take care