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.

Loop powered pulse output circuit.

Status
Not open for further replies.

stambaughw

Junior Member level 1
Joined
Feb 26, 2014
Messages
17
Helped
0
Reputation
0
Reaction score
0
Trophy points
1
Activity points
189
I'm attempting to design a 4-20mA loop powered pulse output circuit for a sensor. If you look at sample circuit1, I can easily produce a clean signal across the load resistor using a typical current shunt resistor, load transistor, and an op-amp to control the current through the transistor. Unfortunately I need a reference voltage to generate the necessary voltages to drive the op-amp input. As soon as I add any kind of reference as in circuit2, the input stabilization capacitor (C1) kills the signal rise and fall times of the signal across the load resistor. If I reduce this capacitor, the rise and fall times improve but the stability of the reference decreases causing overshoot and undershoot in the signal. My questions is, how can I generate a reasonably accurate reference voltage (1%) that can supply ~3mA of current to the rest of my circuit? I've attached the LTSpice simulations for reference purposes. Also note that I tested using the LT1498 supplied by the loop power with the reference unloaded and I get the same results as circuit 2. I just used appropriate Linear parts for simulation purposes.
 

Sorry, not visible.

Sorry about that. Here they are. I had to put them in a zip file. The file uploader wont allow uploading LTSpice .asc files directly.
 

Attachments

  • simulations.zip
    1.9 KB · Views: 43

Yes you can't upload .asc files here. It's one of the many annoyances this site has as compared to some of the other electronic forums. :bang:

Add a diode (such as a 1N4001) between V2 and C1 (to keep C1 from loading the signal).
Increase C1 to at least 1µF.
See simulation.
I didn't have an LT6654 in my library but it should work the same as the LT1236 I used.

Circuit2.PNG
 

Note that it takes about 15ms for the startup transient to settle
.
Also I just realized that, at those high signal frequencies, a fast signal diode such as a 1N4148 would be better than a slow junction rectifier such as the 1N4001.
 
Last edited:

You can change the extension to.TXT and upload the files.
Please don't forget to include any models which are not included on the LTSPICE software itself.
 

You can change the extension to.TXT and upload the files.
.............
Yes.
Which is an annoying extra step for both the poster and the user that the other forums don't require.
All this website has to do is allow .asc files to be directly downloaded.

Also this site doesn't appear to allow direct cut and paste of pictures to your post.
Instead you have to go through a tedious process of saving the picture to a file and then downloading the file and attaching to your post taking about 4-5 steps.
 

Here's an update to the circuit.
I added the model for the LT6654 and changed the diode to a 1N4148.
I also added R2, R3, and C3 to compensate the op amp response and minimize the overshoot in the current output waveform.
It now seems to take about 10ms to settle after power-on.

Circuit2.PNG
 
Last edited:
You can change the extension to.TXT and upload the files.
Please don't forget to include any models which are not included on the LTSPICE software itself.

That's why I embedded the subcircuit model for the transistor. All of the other models were stock LTSpice assemblies. That's why I didn't include them. I update my LTSpice regularly so maybe the LT models I used are new.
 

Here's an update to the circuit.
I added the model for the LT6654 and changed the diode to a 1N4148.
I also added R2, R3, and C3 to compensate the op amp response and minimize the overshoot in the current output waveform.
It now seems to take about 10ms to settle after power-on.

View attachment 131823

Thanks for the help. I don't know why I didn't think of the diode. The only issue I have with the changes you made is the 5V regulator. I need the circuit to operate somewhere in the 4-4.5V range so a 5V regulator isn't going to work. I'll have to use a lower voltage or adjustable regulator. The reason I used a voltage reference is to also provide an accurate voltage for setting the input voltages required to control the loop current. I doubt the regulator voltage will be accurate enough over temperature to meet my requirements.

- - - Updated - - -

Here's an update to the circuit.
I added the model for the LT6654 and changed the diode to a 1N4148.
I also added R2, R3, and C3 to compensate the op amp response and minimize the overshoot in the current output waveform.
It now seems to take about 10ms to settle after power-on.

View attachment 131823

This is interesting. I updated my circuit to match yours but I'm still getting a pretty significant undershoot compared to your results.

lp-pulse-circuit-2.png
 

......................
This is interesting. I updated my circuit to match yours but I'm still getting a pretty significant undershoot compared to your results.
..................
Actually it's overshoot since it goes to a larger magnitude than the flat portion of the waveform.
(If you reverse the direction of Rload in the circuit you will see a positive going current, as I have in my sim.)

But it is curious that you simulation is different from mine.
Offhand I see no difference between the two circuits.
Upload your .asc file and I'll run it to see if I can duplicate the waveform.
 

Actually it's overshoot since it goes to a larger magnitude than the flat portion of the waveform.
(If you reverse the direction of Rload in the circuit you will see a positive going current, as I have in my sim.)

But it is curious that you simulation is different from mine.
Offhand I see no difference between the two circuits.
Upload your .asc file and I'll run it to see if I can duplicate the waveform.

Here it is. One thing I missed is that the loop current is no longer correct. The loop current now swings from ~5.6ma to ~19.9mA. I'm guessing there is a voltage drop caused by the resistors used to minimize the overshoot which is causing the loop current control voltage issue. I can compensate for this by changing the control voltage levels assuming the op-amp is still within it's operating limits.

FYI, I ran the simulation in both LTSpice IV and XVII and I got the same results.
 

Attachments

  • circuit2.txt
    2.9 KB · Views: 52

I simulated your circuit from post #12 without any changes, in my LTSpice IV and it showed no significant overshoot (see below).
(I did rename it circuit2a to differentiate if from the original).

It's a total puzzle to me why there would be a difference between your sim and mine.

You didn't make any changes to the default Spice settings in the Tools/Control Panel, did you?

Circuit2a.PNG
 

A better designed loop powered circuit would measure the total loop current, e.g. by a shunt resistor in the negative line.
 

I simulated your circuit from post #12 without any changes, in my LTSpice IV and it showed no significant overshoot (see below).
(I did rename it circuit2a to differentiate if from the original).

It's a total puzzle to me why there would be a difference between your sim and mine.

You didn't make any changes to the default Spice settings in the Tools/Control Panel, did you?

View attachment 131832

They are different from the defaults. However, clicking the "Reset to Default Values" doesn't seem to make any difference. If your settings are different, please let me know and I will change mine so they are the same. I would feel better if we got the same results.

spice-settings.png

- - - Updated - - -

A better designed loop powered circuit would measure the total loop current, e.g. by a shunt resistor in the negative line.

What are the advantages measuring the total loop current over putting the current shunt in line with the transistor?
 

Your comment about current deviations made me think that you want exactly defined loop currents, as usual in 4-20 mA circuit. But after reviewing your posts I'm not sure if it's an actual problem that variation of voltage regulator quiescent current is reflected in the loop current.

Similarly, I don't understand what's your specific problem with getting a 7 µs low pass filtered current (by the working of C1) instead of sharp square wave. If you connect a long cable with the some capacitance, the waveform rise time will be affected anyway.
 

@crutschow
Your simulation is different due to the start time.

change > simulation> edit simulation cmd>
time to start saving data...> 0

The circuit power up has a 1ms power up rise time constant due to current and caps being charged up from initial supply power up from 0V.
This controls the ref voltage out and thus the current envelope out.

Does this matter?
 

Your comment about current deviations made me think that you want exactly defined loop currents, as usual in 4-20 mA circuit. But after reviewing your posts I'm not sure if it's an actual problem that variation of voltage regulator quiescent current is reflected in the loop current.

Yes. I do want a reasonably accurate (<= 5%) 4-20mA output waveform. That's why I used a voltage reference instead of a regulator. I'm guessing that is why you suggested putting the shunt resistor in line with the current loop so the total current used by the circuit is included in the feedback loop. The primary drawback with that is the voltage drop created by the shunt resistor increases the minimum operating voltage. I would have to significant lower the shunt resistance (probably <= 10Ω) which makes the control voltages pretty low. I'm trying to keep the minimum operating voltage <= 4.5V and my minimum voltage for the non-loop part of the circuit is 3.5V which only leaves 1V of headroom. When you add up the diode drop, the reference or regulator drop out voltage, and the shunt resistor voltage drop, that's starting to get pretty tight. I haven't added the reverse supply protection diode to the input so that would be another voltage drop.

Similarly, I don't understand what's your specific problem with getting a 7 µs low pass filtered current (by the working of C1) instead of sharp square wave. If you connect a long cable with the some capacitance, the waveform rise time will be affected anyway.

I'm not sure what you are asking me here. Suffice it to say, I want the fastest possible rise and fall times on the output wave forms without a lot of distortion for driving long cable lengths. Typically that is the reason to use loop current outputs rather than voltage outputs.
 

Status
Not open for further replies.

Similar threads

Part and Inventory Search

Welcome to EDABoard.com

Sponsor

Back
Top