I'm simulating a verilogams module.
My simulation ends with an error linked to blowup parameter. As follows:

Error found by Spectre at time 15 ns during transient analysis 'amsAnalysis'.
Signal V(..) exceeds the blowup limit for the quantity V which is 1GV.
If you want signal this large, set the 'blowup' parameter of this quantity to a larger value.

My question is the following:
how and in which file I have to change 'blowup' parameter value?

Thanks in advance for the answers.

I have had to change blowup limits for some HV tranformer modeling work I did a while back.  If you are working inside ADE (Artist) the easiest way I found is to make an external file with the "quantity" spectre statement in it.  For example:

quantityV quantity name="V" blowup=200e+12

Then, pull this file into ADE by choosing: Setup->Simulation Files and then under "definition files" put the path to the external file.  Another way is to pull it in as a model file.  

jbdavid -
Are you sure you've got it right?  The reltol is applied to the signal itself, so the 1GV signal only has to converge to within 1MV (change in the value from iteration to iteration), but if you have normal 1.8V signals, they still have to converge to 1.8mV (unless you're using some funny tolerance option that uses the largest signal to set the tolerance for all nodes).

I think Ken's concern is with the other tolerance: vabstol.  If you have something in the GV range, then "numerical noise" will appear around 1e-15 * 1e9 = 1e-6, which is the default for vabstol.  It's easier to understand with currents: if you're adding 1GA and -1GA, you can't expect it to cancel better than 1e-6, so iabstol of 1pA is way too large.

In my experience, when the blowup voltage is exceeded the problem is rarely the blowup parameter being too low, but is a problem with the behavioral models or the circuit.  So try to fix the models and circuit first.  Only once was the huge magnitude legitimate, but even then there were better alternatives to increasing the blowup limit.  

I was using an electrical variable for dV/dt in a behavioral description of capacitance in a filter:

I = C*dV/dt  

Where V had a rather steep slope and C was about 10 pF.  First I tried to create a nature for

Vdiff = dV/dt

but figured out two alternatives that avoided the blowup altogether:

1. Move C inside the differentiation argument, even though C is constant.  That is, instead of
   C * dV/dt
use
   d(C*V)/dt


2. Use integral instead of differential because it's better behaved.  That is,

V = (1/C) * idt(I) + V_initial

Let me know if this helps.