555 Wizard Bad? v10 Multisim

[chuckyRose]

i just dont get it. i use the 555 wizard to build several 555 circuits i found on the net and almost all of them dont behave like they should when i scope the output in Multisim.

then, i try to use the 555 Wizard to build 555 astable 12Vcc 30Hz 51%duty 10nf. it builds but when i scope it the output voltage of each pulse varies, some are 12V while others are 1.2V.

WHY ???

[lacy]

I don't know what is causing your problem, but I thought I might be able to help by posting the Timer Model that I am using in Multisim 2001. I haven't had any problems with it and I use it fairly often.  This may or may not fix your problem but it couldn't hurt to try. This comes directly from my database and it does work in 2001.

.subckt TIMER 0 2 3 4 5 6 7 8
rn1 8 5 5k
rn2 5 51 5k
rn3 51 0 5k
aop1 %vd(5 6) 56 op
aop2 %vd(2 51) 52 op
.model op limit (gain= 300,     
+ out_upper_limit=5,
+ out_lower_limit=-5,
+ limit_range=1 fraction=true)
aadc1 [56 52] [r s] ADC1
.MODEL ADC1 adc_bridge (in_low= 2.5  in_high = 2.5 rise_delay= 1e-12 fall_delay= 1e-12))
anand1 [r Q2] Q1  nand1
anand2 [s Q1] Q2  nand1
.model nand1 d_nand(rise_delay=1n)
adac1 [q1 q2] [66 62] DAC1
rad3 66 0 1
rad4 62 0 1
aadc40 [4] [40] ADC1
aand [40 Q1] Qb and1
.model and1 d_and(rise_delay=1n)
ainv1 Qb 31 inv1
.model inv1 d_inverter(rise_delay=1e-12)
adac72 [Qb] [72] DAC1
aand310 [40 31] 310 and1  
adac31 [310] [32] DAC1
r30 32 0 1g
b1 3 0 v=v(32)*v(8)/5
r3 3 0 1g
.MODEL DAC1 dac_bridge  (out_low= 0.0 out_high= 5.0 out_undef=0.5)
rad5 72 0 1meg
rdisb 71 72 1
qdis 7 71 0 qdis
.MODEL qdis npn ()
.ends

[chuckyRose]

i'm not familiar on how to add a model to the database. can you tell me how i can import your model?

thanks

[lacy]

This is going to be a long explaination so bear with me.

1) Copy the model as is from the post and save it as a text file.

2) go to Create a Component. Select a name for your IC. Select the footprint (i.e DIP8). Select the number of pins in this case 8. Select analog simulation. Select Single section component.

3) don't worry about the symbol yet. Get to the point where it asks for a model and then paste this one there

4) At the very end, You should have a bunch of tabs up at the top of the last dialog box. Select symbol. Under that select "Load from Database". Load the symbol for the virtual Timer. Exit this by clicking either accept or OK (I doing this from my head and don't have Multsim up)

5) Go down to the little box that shows all your pins. and arrange them in the correct order. 1=gnd 2=trig 3=out 4=rst 5=con 6=thr 7=dis 8=vcc  then go to the "footprint" Tab and arrange the pin there in the same order.  These two steps make sure the component pin to model pin mapping are correct. If these are not arranged correctly strangeness will happen.

6 after all that you can now save your component to your user database and use it.

This may not solve the problem with the wizard as I am unsure if it is using a timer from the master database and whether or not this can be changed by the user. A work around is to use the wizard to construct your circuit and replace that timer with yours.

I hope this helps and solves your problem because at this point I am am out of ideas. Good Luck

[Maxish]

chuckyrose,

you must provide more information if you want users to help you.

attach the .ms10 file, or at the least attached a detailed screenshot, and provide a brief explanation
of the misbehavior.

Alec

[chuckyRose]

Maxish,

here's what i did.

1. downloaded and installed the eval of Multisim v10

2. drop a 555 wizard generated timer onto the page

3. placed a scope probe on pin 3 (the real pin 3, the wizard 555 maps wrong pin #'s)

4. then built same circuit on my breadboard

5. attached a real o-scope to pin 3 and results were different than Multisim

in another post (just look for mine, i only have a few) i posted a screenshot of the Multisim circuit. i also have to note though, the more threads i read on this forum the more it seems to be the case that there are numerous issues with the product.

can anyone tell me if there are any patches for v10 ??

Message Edited by chuckyRose on 04-16-2007 09:51 PM

[Maxish]

Chuckyrose,

Your right in noting that the 555 timer model is not exactly the same as the real world one. This is one of the downsides of simulation!

The actual 555 timer chip contains many transistors, and modeling each and everyone of those transistor is typically impractical
as it will drastically slow down the simulation. And even then, chip manufacturers are ussualy reluctant to provide transistor level
details of their designs. As such, Macro models are used to model most parts, including the 555 timer. Marco models obviously
cannot model all the characteristics of the chip and so often only salient features are included.

The 555 timer in Mutlisim is a very generic model of the 555 timer, capturing only the behavioral details. So for example, if the
actual astable/monostable timing is not correct, that is a big flaw.


For a more accurate model, try searching through the chip designer's website. I found one at TI. Simply add it to your user database with component wizard.

******************************************************************************
* TLC555 TIMER MACROMODEL ****************************************************
****************************************4/1/92*****************************DBB
* REV N/A ********************************************************************
******************************************************************************
*                  COMMON
*                  |  TRIGGER
*                  |  |  OUTPUT
*                  |  |  |  RESET
*                  |  |  |  |  CONTROL
*                  |  |  |  |  |  THRESHOLD
*                  |  |  |  |  |  |  DISCHARGE
*                  |  |  |  |  |  |  |    VDD
*                  |  |  |  |  |  |  |    |
.SUBCKT  TLC555    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


cheers,

Alec

[Euler's_Identity]

"i also have to note though, the more threads i read on this forum the more it seems to be the case that there are numerous issues with the product."

[Chuckle]  Ya think?!

[nestor-sg]

Lets not forget that this is not a blog, this is a technical discussion forum for support. People that are having trouble, or find any problems, will most likely post messages in this public forum than people who do not have any problems at all, NI is providing this public forum in a way to have a transparent communication with its customers, and everybody appreciates this.

While other companies block or hide whatever support issues are encountered in their products, NI customers and NI employees we all find very useful to have this public information available, to better understand a product or to better communicate resolutions among the community. And NI constantly monitors these forums as a way to improve the quality and satisfaction level of its products.

Let's remember what our role and responsibility is when posting messages:

http://forums.ni.com/ni/help_faq#communityrole

http://forums.ni.com/ni/help_faq#myresponsibility

[Euler's_Identity]

So what is the solution to the 555 problem?

I, based on this thread and another, designed a one shot with a 555, using MultiSim.

When the 40kHz clk goes low, the output should go high for a couple of microseconds or so and then go low until the next low of the clk.

If I'm not mistaken, for a 555 o/s, t = RCln(2).

With f = 40kHz, t = 1/f = 25us.  For t=10%, t = 2.5us

Choosing C = 0.001uF,

R = t/(Cln(2)) = 2.5us/(0.001e-6*ln(2)) = 2.5e-6/6.93e-10 = 3.6k.

I chose R=3.3k, which should yield t =  RCln(2) = 3.3k(0.001uF)ln(2) =  2.28us.

Nestor, the MultiSim circuit doesn't work.

I've attached the MultiSim V10 file to this post, but it's attached as a .zip in order to get it to the forum, because the forum doesn't accept .ms10 attachments, yet.  You should be able to just change the suffix to .ms10.

Nestor, I don't know what it's doing, but it doesn't even look like a 555 output.  The 555, in this configuration, should immediately slam high whenever the clk goes low and causes a valid trigger of the 555.  At startup the clk is high, so the output should remain low for 12.5us and then go high for roughly 2.2us (when the clk goes low, triggering the 555) and then drop low again awaiting the next low clk.  However, what I'm seeing is the output charging, sort of like a capacitor charging, while the clock is starting high.  Hence, it's wrong right from the start.

I look forward to seeing your solution Nestor.  Thanks!