LTspice issues.
in [Design]
|
From: Jamie on 21 Feb 2010 11:30 pimpom wrote: > Jamie wrote: > >> I don't use LTspice a lot how ever, recently I have been >>poking >>around with a simple buck circuit that just does not seem to do >>in >>spice as it does in real life. I can put those little things >>aside >>how ever, I do have a problem when changing values and then >>exec the >>sim. It pops up with an error stating something on the line of >> "Step size to small x.xxxxxx xxxxxx, error at NC_01" >> >> that may not be the exact message but it's close.. >> >> This can happen just about any where on any component I change >>the >>value on. To fix the problem, I decreas/increase the value by >>1. >> >> For example: >> If change an inductor to 150uf, it didn't like that. I >>could >>go larger or smaller, but I found that all I needed to do was >>to >>add 1 or subtract 1 to make the sim happy. >> >> This does not happen in just inductors, it happens with R's >>caps >>etc.. >> >> Any one have something on that? > > > I don't have an answer but I get similar errors from time to > time. I haven't been using LTSpice for very long either. When the > "error at...." message comes up, it's usually when I forget to > complete a connection and leave a node open. It may also happen > when one makes a connection that LTSpice doesn't understand. > > I have even less clue about the "Step size too small" thing. > Until someone with more insight comes along to enlighten us, I > surmise that it happens when certain combinations of circuit > arrangement, component values and signal and measurement > parameters require more complex calculations than LTSpice wants > to attempt. Maybe multiple parasitic oscillations. I don't know. > Just guessing. > > I have come to the conclusion there is a bug in it. Because when I receive this error, changing a value enough to make it happy allows a SIM operation. Then after a SIM run, I can go back and change that same component to the value I had that generated the error to which it will then exec the SIM with no problems. Since I do a lot of coding my self, I see this as an initiation problem of variables or something of that sort on start up!. I don't recall seeing this problem before the last update that was done. But then again, I'm getting old and memory loss maybe an issue :)
From: Jamie on 21 Feb 2010 11:59 Helmut Sennewald wrote: > "Jamie" <jamie_ka1lpa_not_valid_after_ka1lpa_(a)charter.net> schrieb im > Newsbeitrag news:Yb0gn.1532$mn6.304(a)newsfe07.iad... > >> I don't use LTspice a lot how ever, recently I have been poking around >>with a simple buck circuit that just does not seem to do in spice as it >>does in real life. I can put those little things aside how ever, I do >>have a problem when changing values and then exec the sim. It pops up with >>an error stating something on the line of >> "Step size to small x.xxxxxx xxxxxx, error at NC_01" >> >> that may not be the exact message but it's close.. >> >> This can happen just about any where on any component I change the >>value on. To fix the problem, I decreas/increase the value by 1. >> >> For example: >> If change an inductor to 150uf, it didn't like that. I could >>go larger or smaller, but I found that all I needed to do was to >>add 1 or subtract 1 to make the sim happy. >> >> This does not happen in just inductors, it happens with R's caps >>etc.. >> >> Any one have something on that? > > > > Hello Jamie, > > If the simulator stops with "time step too small", you should try some > options to help the solver. > > 1. > > .tran 20m > > Set a small time step in .TRAN , e.g 100n if you have a 100kHz switching > frequency. > > .tran 0 20ms 0 100n > > If it alreay fails at the beginning, you should try with the > option "startup" in the .TRAN command. > Sometimes additional ".nodeset" will help to get the simulation > started. > > .tran 0 40ms 0 100n startup > > > > I prefer to continue as shown below. > > 2.. > > Control Panel -> SPICE -> Reset to default > Control Panel -> Hacks -> Reset to default > > There are some options which can be helpful. Try either one, > some or all in combination. > These are SPICE directives which you place in your schematic. > > .options gmin=1e-10 > .options abstol=1e-10 > .options reltol=0.003 > > 3. > > If that fails, you could try with the Alternate solver. > Therefore don't use any option from above orr set them to their default > values. > > > Control Panel -> SPICE -> Reset to default > Control Panel -> SPICE -> Solver: Alternate > > The default values: > .options gmin=1e-12 > .options abstol=1e-12 > .options reltol=0.001 > > > > > 4. > > If it still fails, go back to the normal solver. > > Control Panel -> SPICE -> Solver: Normal > > Use the following only as the last option, because it can have a > lot of side effects, especially if you have used a larger value > for cshunt. > > .options cshunt=1e-15 > > This adds a capacitor with 1fF from every node to GND. > I wouldn't go higher than 1e-14. > > You should also use a combination of these options as in 2) in this case. > .options gmin=1e-10 > .options abstol=1e-10 > .options reltol=0.003 > > > Best regards, > Helmut > > > As I indicated in another message, I found that after I make the SIM happy, I run a SIM and if I change the values back to where they were that caused the problem, I can rerun SIM with no issues ;/ Something is wrong with the software. A initiation problem perhaps? BTW. I do use the options in the control panel to make it nearest to real world operation as possible. Nice features btw and still learning what most of them do, good thing there are docs :) I tried a combination of things and no matter what I did, once the error was there, it just wasn't going to start. This error takes place at the very beginning. It does not happen once the annalistic data starts collecting. Who knows, maybe one day I'll track it down..
From: Jamie on 21 Feb 2010 12:01 Wimpie wrote: > On 21 feb, 03:02, Jamie > <jamie_ka1lpa_not_valid_after_ka1l...(a)charter.net> wrote: > >> I don't use LTspice a lot how ever, recently I have been poking around >>with a simple buck circuit that just does not seem to do in spice as it >>does in real life. I can put those little things aside how ever, I do >>have a problem when changing values and then exec the sim. It pops up >>with an error stating something on the line of >> "Step size to small x.xxxxxx xxxxxx, error at NC_01" >> >> that may not be the exact message but it's close.. >> >> This can happen just about any where on any component I change the >>value on. To fix the problem, I decreas/increase the value by 1. >> >> For example: >> If change an inductor to 150uf, it didn't like that. I could >>go larger or smaller, but I found that all I needed to do was to >>add 1 or subtract 1 to make the sim happy. >> >> This does not happen in just inductors, it happens with R's caps >>etc.. >> >> Any one have something on that? > > > Hello Jamie, > > In addition to the good tips of Helmut, you may check your circuit for > unrealistic components. A real inductor has loss that you can model > with resistors and capacitors. > > To increase the simulation speed and/or solve convergence problems, > you can add a resistor in parallel with problematic inductors. You may > add a capacitor in series with the parallel resistor when the effect > on circuit behavior is too large. > > Good luck with getting your simulation to run! > > Wim > PA3DJS > www.tetech.nl > without abc, PM will reach me. Thanks. But toggling the values between SIMS does not explain why I can get it to SIM with the values that originally generated the problem. Oh well. One day I may find out the issue.
From: Helmut Sennewald on 21 Feb 2010 11:45 "Jamie" <jamie_ka1lpa_not_valid_after_ka1lpa_(a)charter.net> schrieb im Newsbeitrag news:ckdgn.25708$K81.23606(a)newsfe18.iad... > Helmut Sennewald wrote: > >> "Jamie" <jamie_ka1lpa_not_valid_after_ka1lpa_(a)charter.net> schrieb im >> Newsbeitrag news:Yb0gn.1532$mn6.304(a)newsfe07.iad... >> >>> I don't use LTspice a lot how ever, recently I have been poking around >>> with a simple buck circuit that just does not seem to do in spice as it >>> does in real life. I can put those little things aside how ever, I do >>>have a problem when changing values and then exec the sim. It pops up >>>with an error stating something on the line of >>> "Step size to small x.xxxxxx xxxxxx, error at NC_01" >>> >>> that may not be the exact message but it's close.. >>> >>> This can happen just about any where on any component I change the >>>value on. To fix the problem, I decreas/increase the value by 1. >>> >>> For example: >>> If change an inductor to 150uf, it didn't like that. I could >>>go larger or smaller, but I found that all I needed to do was to >>>add 1 or subtract 1 to make the sim happy. >>> >>> This does not happen in just inductors, it happens with R's caps >>>etc.. >>> >>> Any one have something on that? >> >> >> >> Hello Jamie, >> >> If the simulator stops with "time step too small", you should try some >> options to help the solver. >> >> 1. >> >> .tran 20m >> >> Set a small time step in .TRAN , e.g 100n if you have a 100kHz switching >> frequency. >> >> .tran 0 20ms 0 100n >> >> If it alreay fails at the beginning, you should try with the >> option "startup" in the .TRAN command. >> Sometimes additional ".nodeset" will help to get the simulation >> started. >> >> .tran 0 40ms 0 100n startup >> >> >> >> I prefer to continue as shown below. >> >> 2.. >> >> Control Panel -> SPICE -> Reset to default >> Control Panel -> Hacks -> Reset to default >> >> There are some options which can be helpful. Try either one, >> some or all in combination. >> These are SPICE directives which you place in your schematic. >> >> .options gmin=1e-10 >> .options abstol=1e-10 >> .options reltol=0.003 >> >> 3. >> >> If that fails, you could try with the Alternate solver. >> Therefore don't use any option from above orr set them to their default >> values. >> >> >> Control Panel -> SPICE -> Reset to default >> Control Panel -> SPICE -> Solver: Alternate >> >> The default values: >> .options gmin=1e-12 >> .options abstol=1e-12 >> .options reltol=0.001 >> >> >> >> >> 4. >> >> If it still fails, go back to the normal solver. >> >> Control Panel -> SPICE -> Solver: Normal >> >> Use the following only as the last option, because it can have a >> lot of side effects, especially if you have used a larger value >> for cshunt. >> >> .options cshunt=1e-15 >> >> This adds a capacitor with 1fF from every node to GND. >> I wouldn't go higher than 1e-14. >> >> You should also use a combination of these options as in 2) in this >> case. >> .options gmin=1e-10 >> .options abstol=1e-10 >> .options reltol=0.003 >> >> >> Best regards, >> Helmut >> > As I indicated in another message, I found that after I make the SIM > happy, I run a SIM and if I change the values back to where they were that > caused the problem, I can rerun SIM with no issues ;/ > > Something is wrong with the software. A initiation problem perhaps? > > BTW. > I do use the options in the control panel to make it nearest to > real world operation as possible. Nice features btw and still learning > what most of them do, good thing there are docs :) > > I tried a combination of things and no matter what I did, once the error > was there, it just wasn't going to start. This error takes place > at the very beginning. It does not happen once the annalistic data starts > collecting. > > Who knows, maybe one day I'll track it down.. > Hello Jamie, Can you send me one example for trying? Best regards, Helmut
From: Helmut Sennewald on 21 Feb 2010 11:57 "Jamie" <jamie_ka1lpa_not_valid_after_ka1lpa_(a)charter.net> schrieb im Newsbeitrag news:ckdgn.25708$K81.23606(a)newsfe18.iad... > Helmut Sennewald wrote: > >> "Jamie" <jamie_ka1lpa_not_valid_after_ka1lpa_(a)charter.net> schrieb im >> Newsbeitrag news:Yb0gn.1532$mn6.304(a)newsfe07.iad... >> >>> I don't use LTspice a lot how ever, recently I have been poking around >>> with a simple buck circuit that just does not seem to do in spice as it >>> does in real life. I can put those little things aside how ever, I do >>>have a problem when changing values and then exec the sim. It pops up >>>with an error stating something on the line of >>> "Step size to small x.xxxxxx xxxxxx, error at NC_01" >>> >>> that may not be the exact message but it's close.. >>> >>> This can happen just about any where on any component I change the >>>value on. To fix the problem, I decreas/increase the value by 1. >>> >>> For example: >>> If change an inductor to 150uf, it didn't like that. I could >>>go larger or smaller, but I found that all I needed to do was to >>>add 1 or subtract 1 to make the sim happy. >>> >>> This does not happen in just inductors, it happens with R's caps >>>etc.. >>> >>> Any one have something on that? >> >> >> >> Hello Jamie, >> >> If the simulator stops with "time step too small", you should try some >> options to help the solver. >> >> 1. >> >> .tran 20m >> >> Set a small time step in .TRAN , e.g 100n if you have a 100kHz switching >> frequency. >> >> .tran 0 20ms 0 100n >> >> If it alreay fails at the beginning, you should try with the >> option "startup" in the .TRAN command. >> Sometimes additional ".nodeset" will help to get the simulation >> started. >> >> .tran 0 40ms 0 100n startup >> >> >> >> I prefer to continue as shown below. >> >> 2.. >> >> Control Panel -> SPICE -> Reset to default >> Control Panel -> Hacks -> Reset to default >> >> There are some options which can be helpful. Try either one, >> some or all in combination. >> These are SPICE directives which you place in your schematic. >> >> .options gmin=1e-10 >> .options abstol=1e-10 >> .options reltol=0.003 >> >> 3. >> >> If that fails, you could try with the Alternate solver. >> Therefore don't use any option from above orr set them to their default >> values. >> >> >> Control Panel -> SPICE -> Reset to default >> Control Panel -> SPICE -> Solver: Alternate >> >> The default values: >> .options gmin=1e-12 >> .options abstol=1e-12 >> .options reltol=0.001 >> >> >> >> >> 4. >> >> If it still fails, go back to the normal solver. >> >> Control Panel -> SPICE -> Solver: Normal >> >> Use the following only as the last option, because it can have a >> lot of side effects, especially if you have used a larger value >> for cshunt. >> >> .options cshunt=1e-15 >> >> This adds a capacitor with 1fF from every node to GND. >> I wouldn't go higher than 1e-14. >> >> You should also use a combination of these options as in 2) in this >> case. >> .options gmin=1e-10 >> .options abstol=1e-10 >> .options reltol=0.003 >> >> >> Best regards, >> Helmut >> > As I indicated in another message, I found that after I make the SIM > happy, I run a SIM and if I change the values back to where they were that > caused the problem, I can rerun SIM with no issues ;/ > > Something is wrong with the software. A initiation problem perhaps? > > BTW. > I do use the options in the control panel to make it nearest to > real world operation as possible. Nice features btw and still learning > what most of them do, good thing there are docs :) > > I tried a combination of things and no matter what I did, once the error > was there, it just wasn't going to start. This error takes place > at the very beginning. It does not happen once the annalistic data starts > collecting. > > Who knows, maybe one day I'll track it down.. > Hello Jamie, Maybe you feel it's different, because LTspice nowadays tries with "pseudo transient analysis" to find the operating point when the classic methods failed. Older versions simply started with the transient simulation even without having found an operating point. You could suppress this method with this SPICE-directive. ..options ptrantau=0 Best regards, Helmut
First
|
Prev
|
Next
|
Last
Pages: 1 2 3 Prev: Speaking of high frequency transformer stuff... Next: Repair water damaged Solar Garden Lamp |