12V Automotive Timer Simulation Difficulties
185 20
Dkraemer 3 months ago
Hello everyone, I'm having some difficulty with my simulation. I've read through the documentation (admittedly, not ALL of it) and have made the changes recommended to get the project to simulate. I've worked through a few examples too. So, t<span class="colour" style="color:rgb(85, 85, 85)">his is an old timer used in public safety vehicles. It is no longer in production. Some coworkers have hinted for some time that they'd like to be able to recreate it because it's been such a solid device for so long and they don't want to move to a different device. I have downtime, so I'm taking it on. T<span class="colour" style="color: rgb(85, 85, 85);">his is good practice for me because I've never been good at circuits and want to get better. </span></span> <span class="colour" style="color:rgb(85, 85, 85)"> </span> <span class="colour" style="color:rgb(85, 85, 85)">The DIP switches on the bottom right are intended to change how long the device stays "on", allowing equipment in the vehicle to remain powered. R12 and R13 were added by me after reading through the tutorials. The battery and igniton are both 12V, but the ignition is the trigger so I changed it to a pulse function. I tried changing the battery to a pulse too, just to see and didn't see much change. R9 is the load I created to see if the relay was working. It's supposed to be a T9AS1d12 12V automotive relay from Potter and Brumfield. I was able to find that model in the spice library that, according to EasyEDA's documentation had a spice model but it didn't seem to work, so I changed it to the current one. Which also doesn't work. I had R9 connected to pin 87 and moved it to 87A when I didn't get an output, which I still don't on 87A. </span> <span class="colour" style="color:rgb(85, 85, 85)"> </span> <span class="colour" style="color:rgb(85, 85, 85)">I'm confident my tracing is correct and I've done my best on components. What I'd like to do is simulate the circuit and see if modifying the switch resistors, capacitors and IC will give a more accurate time range. For example, switch #5 on the device is labeled as "1 to 3 hours" of run time. That seems like a wide margin. The voltage probe C1 shows a ramp up to 12V which is what I would expect, but if I close a switch the voltage is very low, which is what I would expect after some time, but there aren't any transients or anything that shows me info up until that point. I also tried a voltage controlled current switch which I gave 8GV at C1 so that's definitely not correct. </span> <span class="colour" style="color:rgb(85, 85, 85)"> </span> I don't know if I can even accomplish this in EasyEDA. We use the "1-3 hours" selection on the device and taking the simulation out that long may be beyond what EasyEDA is capable of? I think the problem is in my voltage sources. I've been playing with it for a few days and I'm at the point where I need some guidance. Can anyone help me? [https://easyeda.com/editor#mode=sim,id=1443b45e818f4012b551070afced3451](https://easyeda.com/editor#mode=sim,id=1443b45e818f4012b551070afced3451)<br> <br> [https://easyeda.com/Dkraemer/timer](https://easyeda.com/Dkraemer/timer)
Comments
andyfierman 3 months ago
Unless they came from the Spice Symbols section of the library, the relay and the 74HC00 symbol do not have spice models associated with them. Please have another careful read through the Simulation Tutorial.
Reply
eetech00 3 months ago
The relay has no spice model ascociated with it. Also, the part number T9AS1d12  is has 1-Form A contact. You've shown a Form C contact. You haven't shown a timer anywhere so you need to add a timer, such as an NE555. The NE555 can drive the relay directly (add a diode across the relay coil to supress back EMF). A pulse voltage source can be used to trigger the timer for the simulation. There are other issues but too many to describe...
Reply
andyfierman 3 months ago
@Dkraemer, I couldn't check yesterday on my phone but the 74HC00 is a spice symbol so it has a model associated with it so that's OK. The relay does not so try using this one: ![image.png](//image.easyeda.com/pullimage/iw9w9VOM8rbS9x1gJej89MG3lLWZy6Bm7Wg2DEvj.png)
Reply
andyfierman 3 months ago
@eetech00, I don't think Dkraemer is trying to redesign the circuit at the moment. At present the stated aim is to model and simulate the original circuit, maybe modifying it later. I haven't tried simulating it with the replacement relay but AFAIK the original circuit is the timer itself: there is no "missing" 555 timer.
Reply
andyfierman 3 months ago
@Dkraemer, "...a T9AS1d12 12V automotive relay from Potter and Brumfield. I was able to find that model in the spice library that, according to EasyEDA's documentation had a spice model..." Could you point to where you found that because there is no T9AS1d12 in the spice symbol library. Could you also write some notes about how you think the circuit is supposed to work because the way you have drawn the schematic is a biy hard to follow when you don't know quite what it is supposed to be doing. Thanks.
Reply
eetech00 3 months ago
@andyfierman I think you've made some assumptions. The user hasn't posted the original circuit. Only a representation of what is thought to be the circuit. It would be good if they did post the orignal design or specifications document. That way we could simulate it correctly. I never said there was a missing 555, I said there was a missing timer (and there is). I simply implied the user could use an NE555 for the simulation even though it could be used in the actual design. I have a relay spice model that will work for the relay in question.
Reply
Dkraemer 3 months ago
@andyfierman you're correct, I'm not trying to redesign it yet. I just want to get it running and then play with it. The device itself IS a timer. I read in the documentation that you can use a user submitted part that they attached spice information to. These models appear in the search results as blue with a tiny "S" which that part does. I'll be able to find that information on Monday. My understanding of the circuit is: "Battery" is connected to the vehicles battery and "Ignition" is connected to ignition. When ignition is activated, capacitor C1 charges up, the BJT turns on allowing power to florlw through the relay. When ignition is off, C1 discharges through a chosen resistor, keeping the BJT on for whatever time constant RC makes. C2 appears to only apply when S1 is selected and charges through C1. This sort of makes sense because S1 is rated for 15 minutes. Something that throws me is that it looks like the BJT is completely bipassed by the resistor network. I've stared at this device for a long time and I'm confident my tracing is correct, unless there's something about the DIP switches I'm not aware of, or a special property of electrolytic capacitors...or maybe my connections on the relay are incorrect somehow? Thanks for helping.
Reply
Dkraemer 3 months ago
@eetech00 this is the tracing of the device. It's old, there isn't an original circuit and there is no documentation. The company is gone and the device is no longer manufactured so there isn't anyone to ask. I've done my best and pretty confident that my traces are correct. I can post pictures of it of you'd like.
Reply
andyfierman 3 months ago
@Dkraemer, Could you post some close up pjotos to show the wiring/pcb?
Reply
andyfierman 3 months ago
@Dkraemer, Just  realised that you have a note that says "Replaced CD4011BE with 74HC00." I realise that you have done that substitution because there is no CD4011 in the spice library but unfortunately, that won't work because the 74HC series is only specified up to an ABS MAX supply voltage of 7V and the EasyEDA models stop working properly just above above that voltage just as a real device would (they draw an enormous supply current as a warning that something is wrong!). See: **7 Limiting values** in: [https://assets.nexperia.com/documents/data-sheet/74HC_HCT00.pdf](https://assets.nexperia.com/documents/data-sheet/74HC_HCT00.pdf)<br> <br> As you are only using the CD4011 as a non-inverting buffer, for simulation purposes a work around for this is to use a single AND2EE_US spice gate from the EELib in the left hand panel. These gates are specified to work up to 18V ABS MAX. Note that I have written a library not just of the 74HC series but also of some 4000 series parts which have been installed into the EasyEDA library but for some reason only the 74HC series spice symbols are available. I do not know why this is but I have asked for it to be fixed since both libraries were uploaded at the same time.
Reply
andyfierman 3 months ago
Another couple of small but significants error are that in spice is case insensitive and: M = m = milli = 1e-3 Meg = meg = Mega = 1e6 [https://docs.easyeda.com/en/Simulation/Chapter3-About-naming-conventions/index.html#About-naming-conventions](https://docs.easyeda.com/en/Simulation/Chapter3-About-naming-conventions/index.html#About-naming-conventions)<br> <br> 'My understanding of the circuit is: "Battery" is connected to the vehicles battery and "Ignition" is connected to ignition. When ignition is activated, capacitor C1 charges up, the BJT turns on allowing power to florlw through the relay. When ignition is off, C1 discharges through a chosen resistor, keeping the BJT on for whatever time constant RC makes.' So the basic function is that the relay coil is energised when the ignition is turned on and stays that way for a set time after the ignition is turned off. Is that correct? What is the load applied to the relay in a real application?
Reply
andyfierman 3 months ago
@Dkraemer, Well done! Your tracing out of the original circuit is spot on. It does exactly what you said. And but for a few rookie errors, it works in simulation. You might like to have a look and a play with this: [https://oshwlab.com/andyfierman/timer](https://oshwlab.com/andyfierman/timer) I think that if you have another run through the Simulation Tutorial and play with the examples in that, you'll get the hang of it now. It's quite long but well worth going through it from start to finish as simulation is a tricky business and although the simulation engine used in EasyEDA is LTspice, building simulations and running them in EasyEDA is not the same as doing it natively in a local installation of LTspice. Have fun! :)
Reply
Dkraemer 3 months ago
@andyfierman Thank you so much for your help! I did wonder about the naming conventions. I tried to find it in the documentation but wasn't successful. I ran through the series capacitor simulations, which were helpful. I'll look at some more this week. I don't know if anyone would know, but I'm curious why the original design would use such a large IC with the connections it had. It's just 2 NAND gates back to back and why bother? Is it that a single device just doesn't exist? I appreciate (and needed!) the compliment. I've picked this up on and off for 2 years and finally decided to finish it. It's been a great challenge and I've learned a lot. I said, I'm bad with circuits. Even being an EE...they're just not my strong suit so pleased that I did it right! With rookie errors, as you said. :) I took a quick look at the simulation you linked. It seems a lot of things were changed? I'll dive into it in more depth tomorrow. Hopefully I'll be able to understand it and why you made the changes that you did. (I get changing the parts so spice modelling) Thanks again for all your guidance!
Reply
eetech00 3 months ago
I don't mean to be critical, but if it is true that the required timer duration is "Hours", an RC timer like that shown on the schematic cannot be expected to work with reasonable accuracy. A long duration timing IC, like a CD4060B, will be needed. Anyway, good luck with your project.
Reply
Dkraemer 3 months ago
@eetech00 I agree with you, but I want to try. Can't hurt, right? It's for my own enrichment and a good project to put on my resume. Even if it's simple, it shows I'm making an independent effort to gain new skills and challenge myself on my weak points. I could whip something like this up with a small microcontroller fairly easily. It doesn't have to be analog.
Reply
eetech00 3 months ago
@Dkraemer Oh...Ok....I wish you had stated that earlier. good luck..
Reply
Dkraemer 3 months ago
@andyfierman In one post above you showed an image of finding a different relay, but it's in (your?) workspace. I don't see anything for relays when I look at the Spice Library. I'm using the online editor because getting a new program installed at my job is a serious headache. Are the functions of the online editor limited or do you just happen to have a selection of saved relays that you've designed? ![image.png](//image.easyeda.com/pullimage/CkJuRQGuNDpMnUPlrHaFJ4xr2HgUGrdZnxy2P3Au.png)
Reply
andyfierman 3 months ago
The relay is in the User Contributed library. I create a lot of Schematic and Spice Symbols (and their associated models) and Footprints but it is a bit of a pain to move them into the System Library so it takes me a while to move them all into there. So...for the moment, if you see a Schematic or Spice Symbol or a Footprint with my name as owner than that should be OK to use. If you do find an error in any of them, please right click and do Report Error and that will get back to me to fix it.
Reply
Dkraemer 3 months ago
@andyfierman Thanks for letting me know. Since your simplified schematic works, I tacked on the switches as illustrated: ![image.png](//image.easyeda.com/pullimage/ra5NwGi3t53EkCNOxh5yYJa7g5n7CEkuPKigzLcC.png) The names got messed up while I was bouncing around between versions. 2 things: 1.) Closing S15 shows the output going on forever. I believe this is because C3 and C4 are bouncing 6v back and forth. I tried adding a resistor in series with S15 but Relay Out is still held high forever. I tried adding a high value resistor to ground above C4 and one in parallel with C3 but both options resulted in a very Relay Out voltage. I don't know how to mitigate this. I thought perhaps it was an issue with how switches are modeled as specified in the simulation, but I don't know if that's applicable to this situation because I already have output node resistors. The device indicates that S15 should give 15 minutes of run time. 2.) Sometimes I get this error: ![image.png](//image.easyeda.com/pullimage/2ZXtXDsm91TvjE280yk6FnHkYjJMy4gChxhlMeDi.png) I thought it was originally only happening with S10 but if I change the simulation time to 7200, then S10, S12 and S14 fail. S13, 9 and 11 work. Any idea what this could be? It seems dependent on the length of the transient test.
Reply
Dkraemer 3 months ago
Ok, I managed to get S12 working. There appeared to be a connection issue to ground. Even though there was the red node connection circle, I guess it wasn't perfect? It works. I removed C3 since it only operates S15 and I figured C4 could handle it. Is there any reason this could be a bad idea? I attached a 400K resistor to S15. I removed S11 since I couldn't get it to work and I don't think it's necessary. We never used it anyway. Also updated the component names. Updated: [https://oshwlab.com/project/publish/65997925d5964d8fb61c7dc74e606c19#](https://oshwlab.com/project/publish/65997925d5964d8fb61c7dc74e606c19#)
Reply
Login or Register to add a comment
goToTop
svg-battery svg-battery-wifi svg-books svg-more svg-paste svg-pencil svg-plant svg-ruler svg-share svg-user svg-logo-cn svg-double-arrow