PLL不能后仿问题，急啊

初始化VCO的控制电压为0V，前仿真可以正确运行，但是后仿一直卡在数据出来之前那个状态，不能继续往下进行；但是我取消控制线上的电压初始化后，却可以正确的往下进行！
请问这是怎么一回事啊，等了好久都没有仿真数据出来！只能不初始化了么?
刚刚看了下，就是卡在这里：
Trying homotopy = gmin for nodests;
Trying homotopy = source for  nodests;
Trying homotopy = dptram for nodests;
再往下就不能动了！

你把初始电压改变下呢?
你后仿真网表是不是太大了?

    是啊，网表很大，大概十几M的样子，寄生参数很多啊。昨晚上跑了一晚上，最后出现了ERROR：

Trying `homotopy = gmin' for nodesets.
Trying `homotopy = source' for nodesets.
Trying `homotopy = dptran' for nodesets.
Trying `homotopy = ptran' for nodesets.
Trying `homotopy = arclength' for nodesets.
Error found by spectre during DC solution estimation, during IC analysis,
        during transient analysis `tran'.
    There were 7 attempts to find the DC solution. In 1 of those attempts, a
        signal exceeded the blowup limit of it's quantity. The last signal that
        failed is V(I0.I4|I3|NM3:int_s) = 1.60081 GV, for which the quantity is
        `V' and the blowup limit is (1 GV). It is possible that the circuit has
        no DC solution. If you really want signals this large, set the `blowup'
        parameter of this quantity to a larger value.
Trying `homotopy = gmin' for initial conditions.
Trying `homotopy = source' for initial conditions.
Trying `homotopy = dptran' for initial conditions.
Trying `homotopy = ptran' for initial conditions.
Trying `homotopy = arclength' for initial conditions.
Error found by spectre during IC analysis, during transient analysis `tran'.
    There were 7 attempts to find the DC solution. In 1 of those attempts, a
        signal exceeded the blowup limit of it's quantity. The last signal that
        failed is V(I0.I4|I3|NM3:int_s) = 1.60081 GV, for which the quantity is
        `V' and the blowup limit is (1 GV). It is possible that the circuit has
        no DC solution. If you really want signals this large, set the `blowup'
        parameter of this quantity to a larger value.
    No DC solution found (no convergence).

你抽取网表的时候是怎么选的?RC都抽吗?还是只抽C?
如果RC都抽的话，最小的R和C给了多少

    RC都抽的。我没有改设置，都是默认值！您觉得是抽取参数的时候，设置的不对是吧?

你可以只抽C或者RC都抽.
默认值可能都太小了，比如Rmin=0.001ohm, Cmin=0.01fF.
改成Rmin=0.1ohm, Cmin=1fF,
这样抽取的后仿网表文件会小些。
仿真时，你可以先看能不能快速的跑起来（比如power supply设定固定值，vco control voltage设置成最终稳定值附近），如果能跑起来，就是那进度条开始出现....的时候，再加你需要的激励。
不然等过了N长时间，就像你开始列出来那几条信息一样，还是跑不下去，时间就浪费了。

    好的啊，谢谢了！我再试试！

申明：网友回复良莠不齐，仅供参考。如需专业解答，请学习本站推出的微波射频专业培训课程。