1. LTspice
  2. Теми

Electrical Stimulation Unit - Simulation Question

 

Hello all,
 
I just uploaded a zip file containing my schematic for an electrical muscle stim unit along with a picture of the schematic I found in this website: https://www.electroschematics.com/electronic-muscle-stimulator/.
 
I am not trying to build this and use it on myself or anyone else. I am part of a senior design team at my university and one of our goals is to design (not necessarily build) an electrical stimulation unit. I am trying to learn and understand how this DUY unit works so that I can begin designing for our specific parameters. Our main concerns are to have a biphasic waveform (as my understanding goes, we need a net charge of 0 to prevent burns as) and preventing DC Offset. I am most concerned about having the right waveform though.
 
Our program doesn't go in depth into transistors or transformers, so i am not very familiar on how to troubleshoot errors with those. I made my transformer have a 1:10 ratio just to try things out. Additionally, I used a NE555 instead of a 7555. I just dont understand why there voltage/current at the collector of transistor 2 is basically 0, and no current is detected at the electrodes (E1 & E2).
 
The file is called EMS_Circuit.zip.
Thank you all for your time,
Joseph
 

NE555: This is very similar indeed to the 7555, so you can safely use it.

Transistor 2: The collector current is very short pulses of about 112 mA. You can plot it to see the pulses.

E1 and E2: You cannot have a floating circuit in LTspice(any SPICE), because there is no reference to measure voltages from. If you earth/ground E2, you can plot the voltage waveform at E1, very short 32 V pulses. There is another way, without grounding E2. From the Help, under Data trace selection: It is also possible to point at voltage differences with the mouse. You can click on one node and drag the mouse to another node. You will see the red voltage probe at the first node and a black probe on the second. This allows you to differentially plot voltages:

On 2024-12-02 18:04, roolipks via groups.io wrote:
Hello all,
 
I just uploaded a zip file containing my schematic for an electrical muscle stim unit along with a picture of the schematic I found in this website: https://www.electroschematics.com/electronic-muscle-stimulator/.
 
I am not trying to build this and use it on myself or anyone else. I am part of a senior design team at my university and one of our goals is to design (not necessarily build) an electrical stimulation unit. I am trying to learn and understand how this DUY unit works so that I can begin designing for our specific parameters. Our main concerns are to have a biphasic waveform (as my understanding goes, we need a net charge of 0 to prevent burns as) and preventing DC Offset. I am most concerned about having the right waveform though.
 
Our program doesn't go in depth into transistors or transformers, so i am not very familiar on how to troubleshoot errors with those. I made my transformer have a 1:10 ratio just to try things out. Additionally, I used a NE555 instead of a 7555. I just dont understand why there voltage/current at the collector of transistor 2 is basically 0, and no current is detected at the electrodes (E1 & E2).
 
The file is called EMS_Circuit.zip.
Thank you all for your time,
Joseph
-- 
OOO - Own Opinions Only
Best Wishes
John Woodgate
Keep trying

Virus-free.www.avg.com
 
Змінено

On Mon, Dec 2, 2024 at 01:09 PM, <roolipks@...> wrote:
I just dont understand why there voltage/current at the collector of transistor 2 is basically 0, and no current is detected at the electrodes (E1 & E2).
I suspect something is wrong with your 1N4007 diode model.  I don't have a 1N4007 model in my regular library, so I had to either use the default diode "D" in its place, or substitute my own 1N4007 model.
 
  • Your simulation had rather small voltage (picovolts) at V(N003) and current Ic (picoamps) through transistor T2.
  • My simulation with diode "D" has V(N003) peaking at -315 V, and Ic reaching 114 mA.
  • My simulation with my substitute 1N4007 model has nearly the same voltage and current as with "D".
 
I conclude that your 1N4007 model is "bad".  Perhaps it has far too much junction capacitance.  Where did your 1N4007 model come from?  Can you locate and upload it?
 
Regarding the output pins at E1 and E2, you should not be probing those pins themselves.  You should look only at the differential voltage between them, V(E1,E2) or V(E1)-V(E2).  If you probed either pin alone, the waveform would be meaningless.  But I think you got nothing there because the transistor is not able to switch the current through the transformer's primary.
 
Here are a couple of other deficiencies in your schematic:
  • Diode D2 should be a LED, but you did not select any of the actual LEDs, so instead it is a simple switching diode "D".  Right-click on the symbol and pick one of the LEDs.
    • Hint: Click "type" at the top of the list, then scroll up and down until you find the LEDs.
    • Note: It probably does not matter much in the simulation, but it's good to be closer to what it should be.
  • Nets E1 and E2 are floating.  They must not float.  SPICE requires a DC path from every circuit node to ground.  Although floaing E1 and E2 might be correct for the actual hardware, it's not OK for simulations.   Some SPICE simulators refuse to run if you do that.  LTspice flags an error, and it arbitrarily adds a resistor from one of the two nets to ground.
  • I suggest using "ideal" inductors for Lp and Ls.  You used actual products from Bourns and Wurth, which probably can't be turned into a transformer, no matter how hard you try to bend them.  The problem with using those coil products in a simulation, is that they come with some "baggage" that you might not want, including a sizable series resistance, shunt resistance, and shunt capacitance.  They might interfere with the operation of your circuit for generating muscle stimulation pulses.
    • How to fix this:  Delete each inductor, then add new inductors back, and type in the desired inductance value.  DO NOT be tempted to click the "Select Inductor" button, because you would be selecting specific off-the-shelf parts which are fine for some circuits but not for others.
 
Andy
 
 

FYI - You can also fix the two inductors this way:  Right-click on each one, then delete the values for Series Resistance, Parallel Resistance, and Parallel Capacitance.  (Or substitute actual values, if you have them.)
 
When I did that, the peak collector voltage went from -315 to -394 V, and the collector current from 114 to to -126 mA.  So it makes some difference.
 
It's not "right" having Rser=0, but it might be better than the values of those Bourns and Wurth components, in this application.
 
Andy
 
 

Thank you so much both for the detailed responses. Things are much clearer now!
 
Andy,
 
I actually did not upload my own D1 diode. The example I got this schematic from uses the 1N4007 and I found it at the very end of the list (I right clicked the component and then clicked select new diode, then I scrolled to the end and found the 1N4007).
Thank you for pointing out the floating values for the E1 and E2, I am a new LTSpice user and I was not aware of this.
 

By the way, I should have mentioned that I altered Joseph's uploaded file EMS_Circuit.zip, to get rid of the .RAW file that it contained.  As you saw on the group's main webpage, .RAW and .LOG output files usually should not be uploaded.  But in this case, it showed that your (Joseph's) simulations were bad, at the second transistor's collector, and the only thing different from my simulation was the 1N4007.  That's why I concluded that your 1N4007 model is bad.
 
Andy
 
 

Joseph,
 
I think the transformer is backwards in your schematic.  The article says it is a step-down transformer (220 V to 12 V), connected backwards, so it acts as a step-up in the EMS circuit.
 
Not that it matters much, but their ratio is 12:220 or about 1:18, not 1:10.
 
Andy
 
 

1 - 7 з 7