Continue to Site

# Teo wire dimmer

Status
Not open for further replies.

#### Hero999

##### Banned
Two wire dimmer

I was responding to a question over on Electronics Lab, asking whether it's possible to build a PIC-based two wire dimmer, when I had an idea - see attached.

A similar idea could be applied to a motor speed controller or lamp flasher.

It could be used with a PIC (see the link to Electronics Lab above) which could open the door for RF or IR control.

What do you lot think of this idea?

#### Attachments

• Two wire 7555 dimmer.GIF
4.8 KB · Views: 4,431
Last edited:

#### kchriste

##### New Member
Forum Supporter
Looks like it will work. In Lamp flasher mode, particular attention needs to be paid to the value of C1 and the timing period if longer delays are required.

#### audioguru

##### Well-Known Member
I like the bootstrapping action. Then the gate voltage can be high enough for the Mosfet to almost fully turn on.

#### Hero999

##### Banned
Yes, it's bootstrapped.

When Tr1 is off, C1 charges.

When Tr1 is on, C1 powers the circuit and D1 prevents C1 from discharging back into the power supply.

This circuit has one disadvantage: the duty cycle can't be 100% so the lamp is never fully on. If Tr1 is turned on for too long, C1 will discharge below the minimum voltage required to keep the desired current flowing through Tr1.

The maximum duty cycle depends on:

• The current drawn by the load. The higher the current through the load, the faster C1 will charge, meaning the off time can be shorter.
• The current drawn by the dimmer circuit. The lower the current drawn by the dimmer circuit, the slower C1 will discharge, meaning the turn on time can be longer.
• The voltage of the power supply.The higher the power supply voltage the more the voltage across C1 can drop before Tr1 won't be able to carry the desired current.
Increasing the value of C1 won't increase maximum duty cycle or decrease the minimum load current much, it just reduces the ripple voltage on the dimmer circuit's power rail.

With the component values shown it will oscillate at about 200Hz and the maximum duty cycle is 95.5%. The maximum duty cycle is equal to R2/(R1+R2) so this could be increased by reducing the value of R1 but the minimum load current will also increase.

I've just simulated this using Crocodile Clips, a toy simulation package for kids which I use for simple circuits like this. It doesn't have a 7555 model so I used the 555 with a high gain BJT (I set the gain to 1000) and the voltage across C1 is doesn't drop below 5.5V with a load current of 200mA and the component values shown.

With a 7555 the duty cycle could probably be increased to 99% and the load current reduced further. I'll do a simulation using some real software if/when I find a Spice model for the 7555.

Last edited:

#### ericgibbs

##### Well-Known Member
hi hero,
Here you go, enjoy.

#### Attachments

• hero1.zip
8.5 KB · Views: 200
• NE555N_NE555S.zip
2.1 KB · Views: 177
Last edited:

#### Hero999

##### Banned
Here's some formulae:

The average voltage on C1:
[Latex]V_{C1} = \left(Vs- V_{F(D1)} \right) \times \frac{I_{dimmer}}{I_L(1-duty%)}[/Latex]

Idimmer is the current drawn by the dimmer circuit.

Vf(d1) is D1's forward voltage, normally 0.7V for silicon.

The maximum ripple voltage on C1:
$Vripple = \frac{I_{dimmer}}{C \times F}$

Rearranging the above should make calculating the value of C1, the minimum load current and maximum duty cycle easy.

EDIT:
Thanks Eric but I'm after the 7555 model.

Last edited:

#### ericgibbs

##### Well-Known Member
hi,

The 7555 and the TLC555 are almost identical.

#### Attachments

• AAesp07.gif
8.7 KB · Views: 260

#### Hero999

##### Banned
The TLC555 can only source 10mA, the 7555 can source 100mA.

The TLC555, has a maximum supply current of 500µA, the 7555 has a maximum supply current of only 300µA.

I'll give the TLC555 model a go but it'll probably be better with the 7555.

#### ericgibbs

##### Well-Known Member
The TLC555 can only source 10mA, the 7555 can source 100mA.

The TLC555, has a maximum supply current of 500µA, the 7555 has a maximum supply current of only 300µA.

I'll give the TLC555 model a go but it'll probably be better with the 7555.

hi,
If you look in the TLC555test.asc files you will see the circuit schematic with parameters, you could create your version of the 7555.

I have searched without success for a 7555 model.

#### audioguru

##### Well-Known Member
The Cmos 555s are all the same. The Intersil ICM7555, the National LMC555 and the Texas Instruments TLC555.

Only Intersil shows a graph of the "typical" output current.
With a 5V supply the sourcing output current into a dead short is only about 7mA, not more than 100mA like a "normal" 555.
With the 5V supply and a 1V saturation voltage loss the sourcing output current is only about 2.5mA.
With an 18V supply the output current into a dead short is trying to reach only 40mA but then the IC smokes and burns.

With a 5V supply the ICM7555 typically sinks 40mA into a dead short. With the 5V supply and a 1V saturation voltage loss it sinks 18mA.

#### Attachments

• ICM7555 sourcing current.PNG
16.8 KB · Views: 416

#### Hero999

##### Banned
You're right, I didn't look at the datasheets carefully enough.

#### Hero999

##### Banned
hi,
If you look in the TLC555test.asc files you will see the circuit schematic with parameters, you could create your version of the 7555.

I have searched without success for a 7555 model.
Hi Eric,
I've got the files attached.

The only thing I don't like is that the symbol. The pins are laid out as per the IC package and doesn't include pin numbers which make schematic look ugly and hard to follow.

I've made my own symbol which I think looks much better.

How do I specify the model?

I know how to do this in the symbol file, but I want to specify the model after it's been placed into the schematic.

I'm just trying to make it with with the NE555.sub included with LTSpice before I try any of the models you gave me.

The symbol is in the code tags below, save as 555.asy

Code:
Version 4
SymbolType CELL
RECTANGLE Normal -112 -128 112 128
TEXT -23 -84 Left 0 RST
TEXT -26 84 Left 0 GND
TEXT 35 0 Left 0 OUT
TEXT 48 80 Left 0 CV
TEXT 42 -84 Left 0 Vcc
TEXT -83 -80 Left 0 DIS
TEXT -81 0 Left 0 THRS
TEXT -81 80 Left 0 TRG
WINDOW 0 0 -54 Center 0
WINDOW 3 0 47 Center 0
SYMATTR Value 555
SYMATTR Prefix X
SYMATTR Description Generic Symbol for use with subcircuts that you supply.
PIN 0 128 BOTTOM 8
PINATTR PinName 1
PINATTR SpiceOrder 1
PIN -112 80 LEFT 8
PINATTR PinName 2
PINATTR SpiceOrder 2
PIN 112 0 RIGHT 8
PINATTR PinName 3
PINATTR SpiceOrder 3
PIN 0 -128 TOP 8
PINATTR PinName 4
PINATTR SpiceOrder 4
PIN 112 80 RIGHT 8
PINATTR PinName 5
PINATTR SpiceOrder 5
PIN -112 0 LEFT 8
PINATTR PinName 6
PINATTR SpiceOrder 6
PIN -112 -80 LEFT 8
PINATTR PinName 7
PINATTR SpiceOrder 7
PIN 112 -80 RIGHT 8
PINATTR PinName 8
PINATTR SpiceOrder 8

#### Attachments

• 555 test.asc
1.1 KB · Views: 142
Last edited:

#### ericgibbs

##### Well-Known Member
hi,
I have copied your listing, I'll give it ago, dont forget I'm still learning LTspice.

#### Hero999

##### Banned
I've simulated the circuit with the ugly model, I hope you can see what I mean: the schematic in my first post is easier to read because of the pin locations on the IC.

It now works up to 99.5% duty cycle with a 200mA load with the TLC555 model.

I reduced the 100µF down to 10µF and it works fine.

One thing I've noticed is that the model has a setting for Vdd. I don't want to have to set it, I want it to be the voltage on pin 8. I ran the simulation, measured the approximate voltage across the 555, changed Vcc to the appropriate value and re-ran it.

Do you know how to remedy this?

#### Attachments

• two wire dimmer LTS sim1.GIF
21.7 KB · Views: 299
• TLC555dim.asc
2.5 KB · Views: 155
Last edited:

#### Hero999

##### Banned
I've RTFM for the TLC model and it seems like the value of Vdd is only used to calculate the output MOSFET on resistance which varies with the supply voltage.

It looks I'm doing it the right way, run the simulation, find out the supply voltage, run it again, paste the calculated supply voltage into the model's properties box and run it again and paste the newly calculated supply voltage into the properties box. The second guess is always pretty accurate.

The on resistance only matters when R1 or R2 are set to low values, when they're both 50k, it doesn't make any difference.

#### ericgibbs

##### Well-Known Member
I've RTFM for the TLC model and it seems like the value of Vdd is only used to calculate the output MOSFET on resistance which varies with the supply voltage.

It looks I'm doing it the right way, run the simulation, find out the supply voltage, run it again, paste the calculated supply voltage into the model's properties box and run it again and paste the newly calculated supply voltage into the properties box. The second guess is always pretty accurate.

The on resistance only matters when R1 or R2 are set to low values, when they're both 50k, it doesn't make any difference.

hi,
I have run your asy file of the hero Mk1 7555 OK, with the original test asc file.

Lets know if you make any other changes.

#### Hero999

##### Banned
What's that you say you've tested the better looking symbol I posted and it worked?

I couldn't get it to work, there must have been somthing I was doing wrong, please enlighten me.

EDIT:

Last edited:

#### ericgibbs

##### Well-Known Member
What's that you say you've tested the better looking symbol I posted and it worked?

I couldn't get it to work, there must have been somthing I was doing wrong, please enlighten me.

EDIT:

This is how I tried it, you must include the sub circuit.

#### Attachments

• hero2.gif
33.9 KB · Views: 225
• hero2_555.asc
6.6 KB · Views: 201

#### Hero999

##### Banned
Yes, it works.

I hope you agree, that the schematic is much easier to follow now.

#### Attachments

• Two wire dim LTspice.GIF
9.5 KB · Views: 290
• TLC555dim.asc
2.3 KB · Views: 151
Status
Not open for further replies.

Replies
2
Views
2K
Replies
3
Views
6K
Replies
7
Views
1K
Replies
27
Views
3K
Replies
6
Views
1K