captab simulation problem

It would help in future if you actually showed the part of the netlist being referred to by the error if an error message is given by spectre. Knowing what is on line 52 would make this easier to debug.

However, the issue is that you have entered capInfo_dc in the Tran Info Other Params. That's not correct - it should be of the form param=value (which is why it is complaining about the lacking = sign). You're entering the analysis name, which appears in the "infoname" field, which is not showing in the version you're using. The infoname field appears in IC617 ISR21 and later (I think). 

Instead of this, just enter the times in the infotimes field, and then on the Misc Tab, check the captab and timed checkboxes. That will then cause it to create a captab info analysis with the settings on the transient options form, and set it to be produced at the infotimes you entered before.

Andrew.

Hello Andrew,  i made this change as shown bellow and it shown the table although there is no time option in this table.
The main thing that i need to  verify in my flipflop that  the current  shown as I1 on the Left latch is stronger the I2 from the right latch.
How  to know what current flows threw the node responsible for I1 and I2 . i dont know what he means by terminals.what should i do to measure the transient current flow in the selected shown bellow nodes?

Thanks

Hello Andrew,  i made this change as shown bellow and it shown the table although there is no time option in this table.
The main thing that i need to  verify in my flipflop that  the current  shown as I1 on the Left latch is stronger the I2 from the right latch.
How  to know what current flows threw the node responsible for I1 and I2 . i dont know what he means by terminals.what should i do to measure the transient current flow in the selected shown bellow nodes?

Thanks

You seem to be mixing up two completely different things here, so let me address them one at a time. If there's no "Select sweep value" choice to pick the time at the top of the capacitance table, it suggests that something isn't right with the setup or you're using an old version (maybe). Which IC subversion are you using? Help->About will tell you. You only showed a portion of the Capacitance Table window (not even the banner) - this conveys useful information that you're omitting. For example, mine shows:

For the current plotting, a terminal is a pin of a device. You can't plot the current in the wires, because the wires are just a physical drawing to represent a common connection for all the device pins connected to a single net. Nets can have voltage, but not current because there's no flow. If you want to measure the currents, you either need to plot the currents through the relevant device pins (probably you'll need to save those currents - maybe save all device currents from the Outputs->Save All form, although if the models are complex you might need to explicitly ask to save the current through each device pin using Outputs->To be Saved->Select on Schematic). You'd then have to add or subtract those currents to get the total in certain branches.

Alternatively, insert an iprobe device (from analogLib) in the wires in the schematic to measure the current through a particular part of the circuit.

Regards,

Andrew.

Hello Andrew ,I have attached my Cadence virtuoso version,and how i defined my captabs i dont get any time variyng option in the table.
Thanks

Andrew Beckett said:

Instead of this, just enter the times in the infotimes field, and then on the Misc Tab, check the captab and timed checkboxes

The above is from my post two weeks ago. You've not checked the timed checkbox, which is why it is not outputting the captab at the times in the infotimes field.

Regards,

Andrew.

Thanks, it works.