|
Could someone tell me how can I model a SRD in LTspice and use that as a component in other circuits? I am new in LTspice and don't have much idea. I am attaching a link to a paper.
?
I am trying to model SRD according to figure 1 based on equation (1) and then design circuits using SRD as component like figure 2 of the paper. Any help would be much appreciated.
|
On 22/05/2024 23:06, abid wrote:
Could someone tell me how can I model a SRD in LTspice and use
that as a component in other circuits? I am new in LTspice and
don't have much idea. I am attaching a link to a paper.
?
I am trying to model SRD according to figure 1 based on
equation (1) and then design circuits using SRD as component
like figure 2 of the paper. Any help would be much appreciated.
Unfortunately, many of us don't have access to ieeexplore without
paying $$, so we can't see the figure 2 you are referring to. If you
are able to, it would help if you could transcribe it into an
LTspice schematic and upload that, even if you don't have a proper
symbol for SRDs. (I do, though.)
I have done a fair bit of modelling of SRDs. I'll try to dig out
something for you tomorrow, as it's too late here now.
--
Regards,
Tony
|
Thank you for your response. I have uploaded the pictures of the figures and equation. /g/LTspice/album?id=295221
Please let me know if you can't access the photos. I will really appreciate your help regarding SRD modelling. Thanks.
|
We do not encourage posting links to 3rd party
sites, but Research Gate is reliable, so:
\it includes a Spice model, but of course I
don't know how good it is.
On 2024-05-22 22:06, abid wrote:
Could someone tell me how can I model a SRD in LTspice and use
that as a component in other circuits? I am new in LTspice and
don't have much idea. I am attaching a link to a paper.
?
I am trying to model SRD according to figure 1 based on
equation (1) and then design circuits using SRD as component
like figure 2 of the paper. Any help would be much appreciated.
--
OOO - Own Opinions Only
Best wishes
John Woodgate, Rayleigh, Essex
UK
Keep trying
|
Hello,
I saw that paper. This is actually the model I am trying to implement. For the mentioned paper, I don't know how to implement the SDD component in Figure 5. How the equation 2 of that paper can be implemented in the spice model? What are the ports in LTspice? Also, how to use this SRD as a component in other circuits/schematic? These are some of my questions. Thanks.
|
John wrote, "it includes a Spice model, but of course I don't know how good it is."
I am looking for that SPICE model, but I'm not sure if I am seeing it.? Are you referring to the schematic diagram in Figure 3, in the ResearchGate article?? Or maybe Figure 5 (same article)?? Both circuits are missing considerable information, which I think makes them rather useless.
Now mind you, I have not read either article.? I only skimmed them.
I find it peculiar that the two papers share some identical figures, yet there are no authors in common to both papers.
Andy
|
Hi Andy,
My guess is figure 5 is the spice model and figure 3 is the equivalent circuit of the SRD in the ResearchGate article.?
I am not sure how to model the SRD based on the figures given on both the papers and also design the SRD based on the charge equation given on the papers. Also, using SRD to design circuits like figure 2 of the IEEE paper. Any help would be great. Thanks.
|
abid wrote, "I don't know how to implement the SDD component in Figure 5"
This might not answer your question, but a first-look suggests that the "SDD" component might be the circuit in Figure 3.? After saying that, now I will back-track and suggest an alternative.? Both circuits appear to have these components in common: Lp, Rs, Cp.? If these are indeed the same elements with the same values in both figures, then it suggests that the "SDD" component represents only these parts of Figure 3: Cr, Rf, Cf, Vo, and the switch.? The switch might be key to making it model the step-recovery diode.? That is only a guess on my part.
Note that both circuits also appear (exactly the same) in Fig. 1 of the IEEExplore article that started this discussion.? Note the big red arrow in that figure, suggesting that parts (a) and (b) might be the same as one another.
Andy
|
Andy I wrote, "If these are indeed the same elements with the same values in both figures, then it suggests that the "SDD" component represents only these parts of Figure 3: Cr, Rf, Cf, Vo, and the switch.? The switch might be key to making it model the step-recovery diode."
?
Thanks. I also figured that out. But I was wondering how can I design the SDD component in LTSpice? Or should I design the equivalent circuit? I also need to incorporate the charge equation somehow.
|
The SDD element is a
‘Symbolically Defined Device’ that is used in Agilent ADS simulator.
The ADS syntax for the SDD element is definitely not Spice compatible.
Ray Anderson
|
On Wed, May 22, 2024 at 05:46 PM, Ray Anderson wrote:
The SDD element is a
‘Symbolically Defined Device’ that is used in Agilent ADS simulator.
Do you now how to design the SDD in ADS based on the equation and then use that SRD model in other circuits? I could try with the ADS then. Thanks.
|
I have never tried to simulate a SRD using ADS. Apparently there is an Agilent appnote on the topic but I haven’t been able to track it down.
The last time I worked with step recovery diodes was back in the early 1980’s when I was at California Microwave. I wasn’t involved in the SRD frequency multiplier design then, ?but as I recall we had a proprietary simulator written in-house that was used for SRD simulations.
-Ray
|
An image of a spice model for a SkyWorks SRD has been extracted from CVB1031 SRD data sheet and place in the “SRD model and topologies” photo album: /g/LTspice/album?id=295221i haven’t posted a link to the data sheet as it is on an external site and such links are frowned upon in this group. -Ray
|
FYI - There are some step recovery diode models and simulation schematics in our group's Files, from seven years ago.? I refer to these two directories, although beware that some of the uploaded files in them are inconsistent or missing things: Files > z_yahoo > Files sorted by message number > msg_102029 /g/LTspice/files/z_yahoo/Files%20sorted%20by%20message%20number/msg_102029Files > z_yahoo > Files sorted by message number > msg_102029 /g/LTspice/files/z_yahoo/Files%20sorted%20by%20message%20number/msg_102890The .ZIP file in the second of these might be complete.? But it simulates VERY SLOWLY.? I do not know what its original uploader was attempting to do.? Simulating a 200 GHz oscillator for 0.55 seconds seems to me just a little bit odd, and the output file would be ginormous.? Attempting to run that simulation now, I see math errors - voltage values of -1.#IND, which is an error code from the Windows math library.? Some of the file descriptions suggest 400 MHz, but comments on the schematics say 200 GHz, so I would regard them with a great deal of skepticism. But you can see the SPICE model they used for their step recovery diode.? If nothing else, it might be worth studying how it works.? Or maybe not.? Their models are Subcircuits, visible on the schematic sheets.
.SUBCKT SRD1A 1 2
+ Vp=25mV Ip=.220mA Vv=0.125 Iv=0.02mA Vpp=200mV ?C=0.6pF
.param Vt=boltz*(TEMP+273.15)/echarge
BTHE ?1 2 I = Ip*exp(-Vpp/Vt)*(exp(v(1,2)/vt)-1)
BTUN ?1 2 I = Ip*(v(1,2)/Vp)*exp(1-v(1,2)/Vp)
BEXC ?1 2 I = Iv*exp(v(1,2)-Vv)
C 1 2 {C}
.ENDS SRD1A
Andy
|
There is another schematic, from 2006, uploaded by Helmut Sennewald, which also claims to use a step recovery diode.? The diode model in that circuit is an "ordinary" SPICE diode using a .MODEL statement:
.model SMMD840 D(Is=500f N=1.3 Rs=0.22 Eg=1.12 Cjo=1.3p M=0.235 VJ=0.5 Bv=15 Ibv=10u Tt=10n)
I can not confirm any of these models.? I just present them as evidence of what other LTspice users did. Andy
|
I'm sorry, I forgot to include the link to the 2006 schematic file uploaded by Helmut Sennewald, with his step recovery diode.? It is here: Files > z_yahoo > Examples > Educational > step_recovery_diode.asc /g/LTspice/files/z_yahoo/Examples/Educational/step_recovery_diode.ascHis schematic notes say you must use the "Alternate Solver", but it seems to work with the "Normal Solver" too. Andy
|
Could it be 'translated', if it's not too big?
On 2024-05-23 01:45, Ray Anderson
wrote:
The SDD element is a
‘Symbolically Defined Device’ that is used in Agilent ADS simulator.
The ADS syntax for the SDD element is definitely not Spice compatible.
Ray Anderson
--
OOO - Own Opinions Only
Best wishes
John Woodgate, Rayleigh, Essex
UK
Keep trying
|
On Wed, May 22, 2024 at 08:39 PM, Andy I wrote:
I'm sorry, I forgot to include the link to the 2006 schematic file uploaded by Helmut Sennewald, with his step recovery diode.? It is here:
Files > z_yahoo > Examples > Educational > step_recovery_diode.asc
/g/LTspice/files/z_yahoo/Examples/Educational/step_recovery_diode.asc
His schematic notes say you must use the "Alternate Solver", but it seems to work with the "Normal Solver" too.
Is the whole circuit SRD? It's a bit confusing.?
|
On 23/05/2024 10:37, abid wrote:
On Wed, May 22,
2024 at 08:39 PM, Andy I wrote:
I'm sorry, I forgot to include the link to the 2006
schematic file uploaded by Helmut Sennewald, with his step
recovery diode.? It is here:
Files > z_yahoo > Examples > Educational >
step_recovery_diode.asc
/g/LTspice/files/z_yahoo/Examples/Educational/step_recovery_diode.asc
His schematic notes say you must use the "Alternate Solver", but
it seems to work with the "Normal Solver" too.
Is the whole circuit SRD? It's a bit confusing.?
It's just the diode itself that's the SRD. I have uploaded one
of my old schematics that uses the SRD in shunt mode, which is
often more useful than the series mode. It also doesn't use an LC
matching circuit, which makes a wideband design possible. Normally,
SRD comb generators and multipliers tend to be quite narrowband (I/P
PRF).
--
Regards,
Tony
|
abid wrote, " Is the whole circuit SRD? It's a bit confusing," referring to step_recovery_diode.asc from 2006. No, I don't think so.? Only about half of it is. Also, the text is rather small, but you can fix that by starting LTspice with the "-FixUpSchematicFonts" command-line switch.? This schematic pre-dates a change in LTspice's handling of font sizes, which makes them look so small today.? Use "-FixUpSchematicFonts" to update the font sizes. On that schematic, look for the comment text "Diode with parasitics".? The components below that text are:
Those six components represent the SRD.? Well, technically the first four are the SRD, and Cpad1 and Cpad2 are probably the PCB pads to which the SRD connects. All the other stuff to the left of Cpad1 and to the right of Cpad2 are external devices to which the SRD is connected.? It looks like Tshunt is a shorted quarter-wave trap filter, and T1 and T2 just represent traces on the PCB.? Rs is the source impedance and RL is the load. Helmut provided several URLs as comments on the schematic.? It might be worth following those, to see where he got this schematic.? Since it is nearly two decades old, you might need to use the "Wayback Machine" () to retrieve some of them if they are not on the 'net anymore (but hopefully they are). However - Tony is more of an expert on this, so I recommend following his recommendations. Andy
|
Tony Casey
John Woodgate