for my school project i chose "galactic voice changer" (from a 2008 epe magazine ), and as part of my project i need to simulate the functional blocks of the circuit. my problem is that i can't seem able to simulate in circuit maker the oscilator. there should be an output of about 50 mV but what i get is of uV magnitude. the only thing that i changed from the original circuit is a normal 555 timer instead of a cmos555 timer. any help is appreciated !

 

What is ur timer no. Is it a TTL version?

 

what number are you refering to? it's TTL, it's internal structure is made of gates and a flip-flop

 

My circutmaker student version did the same thing until I switched over to the UA555 model.
I suspect that the UA555=TTL, 555=CMOS???

 

the no. on the IC , the timer 555 something.. hello...
gimme a no.

 

The 555 is just a macromodel.
The UA555 is a component model.

Use the component model.

If you try to run either too fast in Circuitmaker, you will have a reduced output from pin 3.

Basically use a range of, 1/400th to 1/1000th of the start-stop time to get sufficient data points without taking a week to run. For example, if you're running an analysis 10mS in duration, use 10uS for step/max step. If you want more resolution, you can always decrease the step/max step. If you want it to run faster, increase step/max step.

Checking the UIC box will help avoid cryptic errors when starting the transient analysis of an astable multivibrator.

 

Ok Sarge, I don't mean to hijack the thread but...
what's the difference between the models?

 

Component model:

*Sngl Timer (Component Model) pkg:DIP8 1,2,3,4,5,6,7,8. pkg:DIP14 1,3,4,6,8,10,12,14. pkg:CAN8 1,2,3,4,5,6,7,8.
.SUBCKT XUA555 99 32 30 19 23 33 1  21
Q4 25 2 3 QP
Q5 0 6 3 QP
Q6 6 6 8 QP
R1 9 21 4.7K
R2 3 21 830
R3 8 21 4.7K
Q7 2 33 5 QN
Q8 2 5 17 QN
Q9 6 4 17 QN
Q10 6 23 4 QN
Q11 12 20 10 QP
R4 10 21 1K
Q12 22 11 12 QP
Q13 14 13 12 QP
Q14 0 32 11 QP
Q15 14 18 13 QP
R5 14 0 100K
R6 22 0 100K
R7 17 0 10K
Q16 1 15 0 QN
Q17 15 19 31 QP
R8 18 23 5K
R9 18 0 5K
R10 21 23 5K
Q18 27 20 21 QP
Q19 20 20 21 QP
R11 20 31 5K
D1 31 24 DA
Q20 24 25 0 QN
Q21 25 22 0 QN
Q22 27 24 0 QN
R12 25 27 4.7K
R13 21 29 6.8K
Q23 21 29 28 QN
Q24 29 27 16 QN
Q25 30 26 0 QN
Q26 21 28 30 QN
D2 30 29 DA
R14 16 15 100
R15 16 26 220
R16 16 0 4.7K
R17 28 30 3.9K
Q3 2 2 9 QP
.MODEL DA D (RS=40 IS=1.0E-14 CJO=1PF)
.MODEL QP PNP (BF=20 BR=0.02 RC=4 RB=25 IS=1.0E-14 VA=50 NE=2)
+ CJE=12.4P VJE=1.1 MJE=.5 CJC=4.02P VJC=.3 MJC=.3 TF=229P TR=159N)
.MODEL QN NPN (IS=5.07F NF=1 BF=100 VAF=161 IKF=30M ISE=3.9P NE=2
+ BR=4 NR=1 VAR=16 IKR=45M RE=1.03 RB=4.12 RC=.412 XTB=1.5
+ CJE=12.4P VJE=1.1 MJE=.5 CJC=4.02P VJC=.3 MJC=.3 TF=229P TR=959P)
.ENDS XUA555

Macromodel:

*Sngl Timer (Macromodel) pkg:DIP8 1,2,3,4,5,6,7,8. pkg:DIP14 1,3,4,6,8,10,12,14. pkg:CAN8 1,2,3,4,5,6,7,8.
.SUBCKT X555 1 2 3 4 5 6 7 8
EREF 15 1 8 1 .5
GSOURCE 8 3 8 26 12.5E-3
GSINK 3 1 26 1 67E-3
VD1 8 27 DC .8
VD2 28 1 DC .85
VREF 30 1 DC 1.2
C1 29 1 700E-15
RREF2 30 1 100E3
RREF 15 1 100E3
ROUT 3 1 100K
R1 6 1 500E9
R2 2 1 500E9
R3 8 5 75E3
R4 5 9 75E3
R5 9 1 75E3
R6 10 11 1E3
R7 13 14 1E3
R8 8 12 150E3
R9 4 8 500E9
R10 20 19 1E3
R11 16 17 1E3
R12 8 18 150E3
R13 8 21 150E3
R14 22 23 1E3
R15 8 26 150E3
R16 24 25 1E3
R19 7 1 500E9
R20 29 26 1E6
D1 1 11 DMOD
D2 12 11 DMOD
D3 12 14 DMOD
D4 1 14 DMOD
D5 18 17 DMOD
D6 1 17 DMOD
D7 18 19 DMOD
D8 1 19 DMOD
D9 21 14 DMOD
D10 21 25 DMOD
D11 1 23 DMOD
D12 18 23 DMOD
D13 26 25 DMOD
D14 1 25 DMOD1
D15 3 27 DMOD
D16 28 3 DMOD
E1 10 1 6 5 1000
E2 13 1 2 9 1000
E3 16 1 15 12 1000
E4 22 1 15 21 1000
E5 24 1 15 18 1000
E7 20 1 4 30 1000
M1 7 29 1 1 MOSMOD
.MODEL MOSMOD NMOS (LEVEL=1 KP=1 VTO=1 RD=5)
.MODEL DMOD D (RS=1E-6)
.MODEL DMOD1 D (RS=1E-6 IS=1E-9)
.ENDS X555

 

i think you were right with the component model, the signal looks different but unfortunatelly i stumbelled on another error:
"Note: starting Gmin stepping
Note: One successful Gmin step
Note: One successful Gmin step
Note: One successful Gmin step
Note: One successful Gmin step
Note: One successful Gmin step
Warning: Gmin step failed
Warning: Gmin stepping failed
Note: starting source stepping
Note: One successful source step
Note: One successful source step
Note: One successful source step
Warning: source stepping failed
doAnalyses: Iteration limit reached
run simulation(s) aborted"

I tried different steping times and durations but it's always the same error.
and i noticed that if i don't check UIC then it doesn't even show the signal, it goes straight to the error.

@ R!f@@ in my project i use TS555CN and because i didn't find it in circuit maker i tried to simulate with a normal 555 timer

 

sorry my bad...

 

connect a 0.01uf cap from pin 5 to ground and try

 

i did connect it but it had no influence, the error persists i think that maybe i didn't give the right values for step time and simulation duration. i tried with 10ms for simulation duration and 100uS, 200uS and 1 ms for steps but it's always the same error

 

The output pin 3 of a 555 switches quickly high and low, not a tiny triangle wave.

 

wait a minute, are u simulating this through multisim

 

wait a minute, are u simulating this through multisim

The OP is using Circuitmaker software package, very similar to multism.

mitza, try checking the UIC box per SgtWookie's instructions.
In my circuitmaker version, its found under:

Simulation -> Analysis Setup -> Transient/Fournier
The UIC box should be on the lower left hand corner.

 

i am simulating in circuitmaker 2000 and i have UIC checked (my checkbox is in the upper side of the window, in the middle) , but still have that error, however it shows me a signal like in the picture attached. if i leave UIC unchecked then that signal doesn't even show. the error is the same in both cases.
i think that maybe i didn't chose the right steping times or simulation time

 

Did it occur for this circuit only. Try another to guarantee ur installation

 

I tried the example supplied with the program and it worked flawlessly. i also reinstalled the program.
i will try and adapt the example circuit to what i need. will be back soon with results.

 

ok, i finally managed to get some good results ! . i modified the example schematic to do what mine does, and i saw that without the buble with .IC in it, it didn't work. i searched it and saw that it's a SPICE instrument. i don't know what it does, but without it the simulation doesn't work. if anyone knows please tell me too . anyhow thank's for helping me, you are a great comunity !

 

Glad to hear that you are making progress

The .IC stands for Initial Condition.
In this case, It tells the software to set the 555 timer's Trig input at a logic 0 when starting its simulation.
Chapter 6 of the users manual does a good job describing Transient Analysis setting. Worth reading.

I did not need it on my software package, but it's a diferent version
Have you tried the UA555 (component model) yet?

Edit:
Here is my waveforms and setting