Query re: datasheet values

Question

I do struggle with making sure I understand what a data sheet is telling me so I'm hoping someone can confirm or otherwise explain my understanding of something. I'm looking at the data sheet for a LTC1624 - http://www.farnell.com/datasheets/1713911.pdf?_ga=2.75130708.790743949.1554834791-441347304.1541859637&_gac=1.136456708.1554891125.EAIaIQobChMI16fD9tLD4QIVz5TtCh3QQglqEAAYAiAAEgKKrvD_BwE

The electrical characteristics state that Vfb feedback current is typically 10nA, max 50nA; Vfb feedback voltage is min 1.178v to max 1.20v.

I'm trying to analyse a circuit, not dissimilar to that shown as an example application in the data sheet, and have built it up in LTSpice. When I simulate this, I can see voltage going into the Vfb pin of 1.15v to 1.3v with peaks of 1.8v falling down to 1.3v (this is a switching regulator at 200Khz). I can see current at the Vfb pin of 14.75nA with peaks of -130nA and 110nA. It will swing from 14nA to -130nA to 110nA back to 14nA in a period of 0.02ms.

This can vary significantly with output load (the above is with a 1kohm load and is more extreme with lower resistance.) If I build the example application in the data sheet the current to the Vfb pin is within the specified range but the voltage is under the minimum level or over the maximum (again, depending upon load.)

My assumption would be that my circuit would be a problem but it's confusing because the example application also simulates outside the specifications. This is when I start to think I'm not interpreting the data sheet information correctly. Could someone proffer some advice?

I've not posted pictures of the circuit or the simulation results because it's more a question of correctly/incorrectly interpret the specifications - obviously I can if it's important/useful enough.

Thanks

Andrew

shabaz · Accepted Answer

Hi Andrew, That's correct regarding the voltage value (The current value indicates what that input pin will take, and so the potential divider must provide that current - that can be done by choosing potential divider resistances such that the current through the potential divider itself is much larger than that to reduce error, but not so great that too much power is wasted. As an example, if the divider ratio was decided to be (say) 1:2 and R1 and R2 were then (say) 10M and 20M respectively that might not be appropriate, but if they were 10k and 20k respectively then that may be more appropriate. But, the datasheet has to be consulted regarding this feedback circuit, often it will suggest what ballpark either R1 or R2 should be in, or there may be an example circuit with values, it's important not to stray too much from that ballpark to prevent instability.

michaelkellett · Answer

Crumbs !!! If I had a spare age or two I could work out what all this is meant to do - is there a description somewhere ? My installation of LTSPice moans that it can't find the 7805 - no matter - if I were modelling this I wouldn't have it in any way The key to simulation is to keep it simple - those // caps don't do anything for you (since they use simple models and don't have even series resistance added). Looks like that entire 7805, LTC1983, 2N3904 chain is just there to provide a roughly constant current (about 20mA) towards ground - for debugging the simulation use a current source. So, if I wanted to understand the LTC1624 and it seemed to do something odd (in simulation), I would first get it into a nice simple model and play with that. Once that is going nicely, start adding the other bits. MK

shabaz · Answer

Hi Andrew, The voltage at that pin can go beyond 1.178..1.2V (this is a tolerance of the internal reference, not really a range), it's easiest to consider it like an input pin - it's a feedback input. The switching regulator will have spikes, the IC cannot respond (i.e. accept feedback) fast enough to completely remove them from the output (and hence there are spikes at the feedback pin too, since that's seeing a representation of the output voltage divided down). The engineer creating the circuit needs to know the datasheet feedback voltage value, so that they can pick the voltage divider values (R1 and R2) so that the Vfb input pin sees 1.178..1.2V when the output is at the desired voltage.

jc2048 · Answer

In case you don't know, you can save a schematic via the clipboard like this. It isn't very obvious the first time you use LTSpice. I then read it into GIMP and export it as a .png file, though you'll probably have your own favourite way of doing that bit. You'll probably get more of a conversation going if there are embedded pictures to look at in your discussion posts rather than links to files on other websites. With regard to the design files, people seem to be able to attach .zip files to blog posts, so maybe try that.

michaelkellett · Answer

Reading data sheets is a bit of an art, and all the manufacturers have their own different ways of doing things.

LT define the FB pin current under "Electrical Characteristics" - these are usually things that the part determines.

The absolute maximum is defined for Vfb (-0.3V -> 2.7V) but they don't define current for anything other than Vfb = 1.8V.

We can tell from the block diagram that it is a high impedance input but that's about it.

We can get an idea of where the current comes from, the voltage on the FB pin changes by 30mV in about 1.5us, and the current during this time is about 158nA.

This is equivalent to a pin to ground capacitance of (I * t)/v = approx 8pF - which seems quite reasonable.

In your circuit there is a 100pF cap in // with this input so the current into that will be much higher.

When worrying about the MOSFET, the Vgs that will hurt it is the Vgs relative to the source, not the Vgs net on the circuit. You can see this by adding a trace V(Vgs) - V(Vsw), and it doesn't go above 6V.

Good luck with you exploration - that's enough distraction for me today - must get back to the job I'm avoiding

MK

michaelkellett · Answer

I had a quick look at the reference model and the data sheet. I put 1000R in series with the FB pin so I could see the current (started with the standard LTC1624 example) And it looks like this: Blue trace is feedback voltage, red is feedback current. If you check the data sheet carefully you will see Note 2 by the IinFB parameter - its says: The LTC1624 is tested in a feedback loop which servos VFB to the midpoint for the error amplifier (VITH = 1.8V) Which indicates that the feedback current will vary in an unspecified way if the feedback is not perfectly in balance ! My plot shows that the average feedback current is about 10nA which is in spec. The shape of the current waveform looks as if there is some capacitance to ground in the model (and that makes sense). LT use LTSpice to design their chips - the models (and LTSpice) are pretty good. MK

Andrew J · Answer

Thanks Jon. My original purpose wasn't to task someone to "please look at this circuit for me and see that it works", which is why I didn't post it originally (I don't want to be one of those sorts of members.) I was really trying to clarify what the data sheet was telling me that I couldn't understand - even the LT application looked odd in simulation against the specs in the data sheet. It's not easy to research that level of specificity (I know, I tried)! I guess conversations evolve along the way (and I appreciate the help that everyone gives as it does so.) Hopefully that makes sense.

Look at that lovely, rich LT Spice interface you got going on there! I use the MacOS version which doesn't have such new-fangled options such as 'copy bitmap to clipboard' It barely has options at all

I was, at some point in the future, going to blog about my experience/journey with all this, including attaching files so I guess the blog interface is different to the discussions interface.

Andrew J · Answer

I hear you - I really didn't want to drag anyone into spending ages debugging this which is why I didn't post it first and was asking about the data sheet principally. It's something I'm working on as part of my own education so I try not to get people to do my work for me, if that makes sense. Sometimes, however, I just run into things I can't get my head around or find information on. With the schematic built in LT Spice it works: I can adjust the load (RLOAD), VCTRL and ICTRL and vary the output in line with expectations at least as far as my limited experience tells me. What I was getting into was some detail of the circuit as part of understanding it further and ensuring that the simulation wasn't hiding anything - for example, as I understand it, LT Spice doesn't flag up things such as over-powering devices. When I was looking at the voltage and current loads against the data sheet of the LTC1624 I was concerned this was one of those 'hidden' things. Essentially, this is a bench power supply based on a design from Linear Technologies: https://www.analog.com/en/design-center/evaluation-hardware-and-software/evaluation-boards-kits/dc2132a.html# That uses a bunch of ICs in a QFN package which I didn't want to get into soldering, frankly, if I moved this forward. There is an alternative build here which uses 'easier' components but based on the same design (not exactly but...) https://www.instructables.com/id/High-Performance-Adjustable-Power-Supply-50-With-O/ What I was aiming for was ensuring that it worked and understanding how: the schematic's BOM is different to the provided LT Spice model that shows 'it works'. I re-created the model (which you have seen) and using the BOM shows me it doesn't, so I've made some slight adjustments, e.g. changing the Mosfet (and now it does simulate correctly at least). Once I got it to a certain point I was then going to look at individual pieces of it and consider alternatives. For example, the 7805, LTC1983 and 2N3904 are just doing what you say and it allows the LT3081s to go to 0v. However, the power drop on the 7805 is a possible concern and I don't need a regulator that is capable of providing 1A there, so I was going to investigate alternatives, perhaps even an alternate power source for that part. As an aside, even if I went further with the LT DC2132a design linked above, I would still have re-created a LT Spice model to get an understanding of how it was working. If you do want to look at it further, I have put the 7805 library and schematic here. Sorry, I forgot those were models I'd downloaded (they came from the LT Spice Yahoo group): https://1drv.ms/u/s!AkgMkSdwBcLBhURMa2Z_QgDaAvPS https://1drv.ms/u/s!AkgMkSdwBcLBhUVL0et2Qom29n82 In terms of, say, your point in respect to the LTC1624 doing something odd in simulation, that was my first thought. So I built up a separate, simple model in LT Spice, based on the example application in the data sheet, but that also looked 'odd' to me as well! I assumed it related to my understanding of/confusion with what the data sheet was telling me: I wasn't inclined to believe that Linear Technologies would put an example into the data sheet that was wrong but I couldn't figure out why, if the data sheet says min/max is X/Y, that the simulation of LT's application was not in that range. At the time, if I saw the results you posted above showing the current swinging from -50nA to 190nA I would also think that might be a concern given the min/max in the data sheet of 10nA/50nA! If I'm honest with myself, I'm still not sure how the data sheet says it isn't a problem! I guess that will come with experience. Hopefully that all makes sense! I really appreciate the input and time, thanks.

michaelkellett · Answer

I've used LTSpice for many years and simulated a good number of switching circuits. I think you are worrying about a detail than may well be unimportant. The transient currents may not be totally accurate for short spikes, and will certainly not be the same in real life (because all the parasitics will be different). If you were to post the LT spice schematic and the model I could run it and make a more informed comment on the issue you report. (Are you using the LT supplied example design as a start point ?) MK

Query re: datasheet values

Top Replies