Continue to Site

Welcome to EDAboard.com

Welcome to our site! EDAboard.com is an international Electronics Discussion Forum focused on EDA software, circuits, schematics, books, theory, papers, asic, pld, 8051, DSP, Network, RF, Analog Design, PCB, Service Manuals... and a whole lot more! To participate you need to register. Registration is free. Click here to register now.

Register Log in

doAnalyses: TRAN: Timestep too small; initial timepoint: trouble with

Status
Not open for further replies.
P

promach

Advanced Member level 4
Joined
Feb 22, 2016
Messages
1,199
Helped
2
Reputation
4
Reaction score
5
Trophy points
1,318
Activity points
11,636
I have created a series, shunt LC bandstop/notch filter.

https://github.com/promach/frequency_trap/tree/9806e6c293463c1eca3b1b5f0c92ac3e76d14f28

Screenshot from 2018-01-28 08-57-56.png Screenshot from 2018-01-28 08-59-02.png Screenshot from 2018-01-28 09-00-11.png

The screenshots above correspond to frequency_trap.net, CMOS_Inverter.net and Gm2.net respectively.

However, when I run "make clean && make" after cloning the project from github, ngspice gave me the following error:

doAnalyses: TRAN: Timestep too small; initial timepoint: trouble with p1-instance m.x1.m4
tran simulation(s) aborted
Click to expand...

Could anyone advise ?

CMOS_Inverter.net

Code: 
* gnetlist -L ../.. -g spice-noqsi -o CMOS_Inverter.net CMOS_Inverter.sch
* SPICE file generated by spice-noqsi version 20130710
* Send requests or bug reports to [email]jpd@noqsi.com[/email]
.subckt INV1 2 1
M4 1 2 Vdd Vdd P1  l=0.4 w=3         m=25
M1 1 2 Vss Vss N1  l=1.2 w=3         m=25
*
*
.ENDS


frequency_trap.net

Code: 
* gnetlist -L ../.. -g spice-noqsi -o frequency_trap.net frequency_trap.sch
* SPICE file generated by spice-noqsi version 20130710
* Send requests or bug reports to [email]jpd@noqsi.com[/email]
Ctest X1.IN Vout 1n      
Vd Vdd GND 'SUPPLY'
Vs Vss GND 0V
.GLOBAL Vdd Vss
.INCLUDE CMOS_Inverter.net
.INCLUDE Gm2.net
.INCLUDE active_inductor.net
.PARAM SUPPLY=3.3v
.options TEMP=25
.MODEL n1 NMOS
.MODEL p1 PMOS
Vtest Vtest GND dc 0
+ac 1
CL GND Gm2.IN 0.07pF      
XGm2 Gm2.IN Gm2.OUT GM2
X1 X1.IN X1.OUT INV1
V_IP_X1 X1.OUT Gm2.IN DC 0V  
V_IP_Gm2 Gm2.OUT X1.IN DC 0V  
Rs Vtest Vout 1e99 ac=1e-6      
.control
op
ac lin 10000 138 200
write frequency_trap.raw
gnuplot vtest db(vtest)
gnuplot vout db(vout)
*plot Vtest Vout
tran 0.1p 400p
plot Vtest X1.IN X1.OUT
setplot
plot i(v.xgm2.v_ip3) i(v.xgm2.v_ip4) i(v.xgm2.v_ip5) i(v.xgm2.v_ip6)
noise v(Vtest) Vtest lin 100 1 10G
setplot noise1
let noise_figure=db(inoise_spectrum)/2-db(2*sqrt(boltz*290*50))
plot noise_figure
.endc


Gm2.net

Code: 
* gnetlist -L ../.. -g spice-noqsi -o Gm2.net Gm2.sch
* SPICE file generated by spice-noqsi version 20130710
* Send requests or bug reports to [email]jpd@noqsi.com[/email]
.subckt GM2 7 3
M4 g3 g3 1 1 P1  l=1u w=3u         
M3 3 g3 2 2 P1  l=1u w=3u         
M5 3 5 4 Vss N1  l=1u w=3u         
M6 g3 7 6 Vss N1  l=1u w=3u         
I2 8 Vss 40uA
I1 9 Vss 40uA
Vb 5 Vss 1.8V
Rs 9 8 500k      
*
*
V_IP6 6 8 DC 0V  
V_IP5 4 9 DC 0V  
V_IP4 Vdd 1 DC 0V  
V_IP3 Vdd 2 DC 0V  
.ENDS
 

Timestep too small
Click to expand...

Examine your timestep value. Increase it by 10x. See if you get the same error. Do this repeatedly and see if it brings success.

initial timepoint: trouble
Click to expand...

As a run begins, assign each capacitor some definite level of charge (0V or any reasonable voltage). Likewise every component for which you left a required parameter blank.
 


Your inverter's width is 3 meters, length is huge too. Simulators can't handle such big relative differences between the devices, maybe this is a reason.
And Rs is 1e99 Ohm? Extremely high, now I am not sure that my processor could calculate with this value anything.
 
Last edited:
@frankrose

Thanks for the micrometer dimension advice.

Correcting the CMOS inverter dimension and changing Rs to 1e-6 during transient help to eliminate the transient simulation error, giving me the following transient simulation voltage plots.

Screenshot from 2018-01-28 21-10-09.png

I have a side question:

For CMOS inverter , why does the input terminal has a higher voltage (approximately 0.3V) compared to output terminal ?
 

Because it is an inverter. When the output is higher, the input is lower and vica-versa. It is natural. To set 1.8V output the input can be lower or higher. Your Gm cell sets the output to 1.8V, but the input is determined by the NMOS/PMOS characteristics.
 

In ngspice, .OP gave me the following:

I am looking at it now. Does anyone have any comments ?


Initial Transient Solution
--------------------------
Node Voltage
---- -------
x1.in 2.09899
vout 0
vdd 3.3
vss 0
vtest 0
gm2.in 1.8
xgm2.g3 2.14857
xgm2.1 3.3
gm2.out 2.09899
xgm2.2 3.3
xgm2.5 1.8
xgm2.4 0.649101
xgm2.6 0.649101
xgm2.8 0.649101
xgm2.9 0.649101
x1.out 1.8
v_ip_gm2#branch 0
v_ip_x1#branch 0
v.xgm2.v_ip3#branch 4e-05
v.xgm2.v_ip4#branch 4e-05
v.xgm2.v_ip5#branch 4e-05
v.xgm2.v_ip6#branch 4e-05
v.xgm2.vb#branch 0
vtest#branch 0
vs#branch 0.00280043
vd#branch -0.00280043
Click to expand...
 

Status
Not open for further replies.

Similar threads

Part and Inventory Search

Welcome to EDABoard.com

Sponsor

Back
Top