• Welcome to our site! Electro Tech is an online community (with over 170,000 members) who enjoy talking about and building electronic circuits, projects and gadgets. To participate you need to register. Registration is free. Click here to register now.

Does this PSPICE netlist look right to you?

Status
Not open for further replies.

Hardwire

New Member
It is from Linear Systems for their SST211 lateral DMOS switch (datasheet: http://www.electro-tech-online.com/custompdfs/2007/04/SST211.pdf)

And this thing just won't act right in Pspice...

I try to switch it on and off with a 0 - 5V signal but it doesn't really want to work.

So I noticed something in the netlist that looked odd:

---------------------------
.MODEL SST211 NMOS ( LEVEL = 7
+VERSION = 3.1 TNOM = 27 TOX = 1E-7
+XJ = 1.5E-7 NCH = 1.7E17 VTH0 = 1.0941063
+K1 = 2.4541877 K2 = -0.05 K3 = 80
+K3B = 0 W0 = 2.5E-6 NLX = 1.74E-7
+DVT0W = 0 DVT1W = 0 DVT2W = -0.032
+DVT0 = 2.2 DVT1 = 0.53 DVT2 = -0.032
+U0 = 537.6815365 UA = 1E-8 UB = 1.998E-18
+UC = 1.31205E-9 VSAT = 8.8E4 A0 = 0.93
+AGS = 0 B0 = 0 B1 = 0
+KETA = -0.047 A1 = 0 A2 = 1
+RDSW = 4E3 PRWG = 0 PRWB = 0
+WR = 1 WINT = 0 LINT = 0
+XL = 0 XW = 0 DWG = 0
+DWB = 0 VOFF = -0.0593033 NFACTOR = 0.2282159
+CIT = 0 CDSC = 1.5E-4 CDSCD = 0
+CDSCB = 0 ETA0 = 1E-7 ETAB = -0.07
+DSUB = 0.56 PCLM = 0.134 PDIBLC1 = 9.934E-5
+PDIBLC2 = 1.013829E-3 PDIBLCB = 0 DROUT = 0.01
+PSCBE1 = 8.456E8 PSCBE2 = 3E-6 PVAG = 0.1405676
+DELTA = 0.13 MOBMOD = 1 PRT = 0
+UTE = -1.5 KT1 = 0 KT1L = 0
+KT2 = 0 UA1 = 4.31E-9 UB1 = -7.61E-18
+UC1 = -5.6E-11 AT = 3.3E4 PHI = 0.7582363
+NQSMOD = 0 WL = 0 WLN = 1
+WW = 0 WWN = 1 WWL = 0
+LL = 0 LLN = 1 LW = 0
+LWN = 1 LWL = 0 CAPMOD = 2
+XPART = 0 CGDO = 1.91225E-9 CGSO = 3.146805E-9
+DLC = 0 DWC = 0 )
*
* W= 889.0um L= 0.5um
--------------------

Last two lines: the dimensions of the channel are commented out? Aren't they supposed to be inside the parenthesis?

I've tried moving the W and L parameters inside the parenthesis, but it still won't simulate correctly.

It's just my luck that the one DMOS switch in all the world that I have to simulate, doesn't work :mad:

Any insight into this will be appreciated.
 

Roff

Well-Known Member
In general, channel width and length are parameters which can be different for each individual MOSFET in a circuit. In your case, all SST211's will have the same values of these parameters. I haven't used Pspice in years, but the NMOS transistor should have a place to enter these parameters, or a way to pass them to it. I think they are shown as comments so you will know what values to enter. They are NOT model parameters.
 

Hardwire

New Member
Ah, okay. The L/W parameters might be declared somewhere in the library, but not actually in the netlist for each device. I'll scroll through the library declarations and see what I can find. Thanks.
 

Optikon

New Member
For a level 7 model, L & W are infact model parameters that can be populated. If left unspecified, they assume default values sometimes specified with .option perhaps (LDEF, WDEF??)

Also, don't rule out that the model might be junk - won't be the first time that's happened. Otherwise, nothing looks wrong with it. Is your circuit doing something goofy to it?
 

Hardwire

New Member
Well I tried modifying the L/W parameters in the OPTIONS menu for "Mosfet" category... but still the darn SST211 doesn't switch. So I did some more digging on this model and found out that other people had the same problem, and someone found a solution but I don't know how to apply it.

From http://groups.google.com.sb/group/s...read/thread/de405f561d1813ae/3f9901943b082847

Someone seems to have corrected the model by "sizing" it correctly with a new template. Apparently, the issue is, in fact, the L/W parameters, but I don't know how to apply the fix they describe below:

link above said:
OK, I found the problem. The bare model is not SIZED.
You need to create a part such that its template is...

MN1 %d %g %s %b SD210 L=0.5u W=889u <<<<

I then get ID = 12mA at VGS = +2.5V, VDS = +2V

And the slope near the origin is 52.6 ohms.
Unfortunately I'm not quite clear on how to do this template stuff. I'll be looking into it, but if anyone has a quick explanation, I'd love to hear it.

I'm e-mailing the author of the google groups reply cited above, so maybe that will help too.
 

Optikon

New Member
Hardwire said:
Well I tried modifying the L/W parameters in the OPTIONS menu for "Mosfet" category... but still the darn SST211 doesn't switch. So I did some more digging on this model and found out that other people had the same problem, and someone found a solution but I don't know how to apply it.

From http://groups.google.com.sb/group/sci.electronics.design/browse_thread/thread/de405f561d1813ae/3f9901943b082847

Someone seems to have corrected the model by "sizing" it correctly with a new template. Apparently, the issue is, in fact, the L/W parameters, but I don't know how to apply the fix they describe below:


Unfortunately I'm not quite clear on how to do this template stuff. I'll be looking into it, but if anyone has a quick explanation, I'd love to hear it.

I'm e-mailing the author of the google groups reply cited above, so maybe that will help too.
That template seems to just set L & W for the instance of SD210 called. To me, that should have the same effect as setting L & W inside the model itself. ????
 

Hardwire

New Member
That's what it looks like to me, too. But when I modify the netlist to include the L W info inside the parenthesis (not commented out) it doesn't fix the problem either.

I e-mailed the guy who responded in the google groups and asked if he could just send me the modified model.
 

Roff

Well-Known Member
L and W are geometry scaling parameters. I don't think Pspice will recognize them inside the model file. I don't use Pspice, so I don't know how to specify L and W for an instance of a MOSFET. Have you tried double-clicking on an instance of the part in your schematic? Does this open the Attribute Editor?
I got the model to run in LTspice, but rDS(on) was about 19 ohms with Vgs=5V, while the datasheet says it should be typically 60 ohms.
In LTspice, when you right-click on the NMOS4 symbol, a dialog box opens which allows you to specify L and W. I also has entries for Ad, As, Pd, and Ps, which are unfortunately not specified in the datasheet. These affect source-to-body and drain-to-body capacitances. I swept these values over what I thought were some typical ranges, and there was no change in the DC sweep curves, as expected.
 

Hardwire

New Member
Ron H said:
L and W are geometry scaling parameters. I don't think Pspice will recognize them inside the model file. I don't use Pspice, so I don't know how to specify L and W for an instance of a MOSFET. Have you tried double-clicking on an instance of the part in your schematic? Does this open the Attribute Editor?
I got the model to run in LTspice, but rDS(on) was about 19 ohms with Vgs=5V, while the datasheet says it should be typically 60 ohms.
In LTspice, when you right-click on the NMOS4 symbol, a dialog box opens which allows you to specify L and W. I also has entries for Ad, As, Pd, and Ps, which are unfortunately not specified in the datasheet. These affect source-to-body and drain-to-body capacitances. I swept these values over what I thought were some typical ranges, and there was no change in the DC sweep curves, as expected.
Bless your heart.

I truly could not see the forest for the trees.

After several minutes I was able to locate the attribute editor, and I was able to change the W and L values for this instance of the part. (Orcad Capture hides the attribute editor in the Part Editor which looks more like a graphics editor instead. And until you poke around in the submenus you can't find it. It SHOULD be a simple double click to change ANY attribute of the part but the Orcad people are evil.)

Thank you so much for the help, Ron H and Optikon!

:) :)

P.S. And now the mosfet switches as it should :)
 
Last edited:

Roff

Well-Known Member
Hardwire said:
Bless your heart.

I truly could not see the forest for the trees.

After several minutes I was able to locate the attribute editor, and I was able to change the W and L values for this instance of the part. (Orcad Capture hides the attribute editor in the Part Editor which looks more like a graphics editor instead. And until you poke around in the submenus you can't find it. It SHOULD be a simple double click to change ANY attribute of the part but the Orcad people are evil.)

Thank you so much for the help, Ron H and Optikon!

:) :)

P.S. And now the mosfet switches as it should :)
I found a reference to the attribute editor while Googling "Pspice manuals" or some such. It must have been an old manual, as it said to double click on the part.
Glad you were finally able to get your sim to run. After looking at the results of my LTspice DC sim, and at the comments of the guys on the forum you referenced (sci.electronics.design), I would not have much confidence in any results that rely on rDS(on) or device capacitance. I know (by reputation) some of the guys that were posting in that thread. They are truly experts, and they were getting results which did not match the datasheet.
What are you using the part for?
 

Hardwire

New Member
Ron H said:
I found a reference to the attribute editor while Googling "Pspice manuals" or some such. It must have been an old manual, as it said to double click on the part.
Glad you were finally able to get your sim to run. After looking at the results of my LTspice DC sim, and at the comments of the guys on the forum you referenced (sci.electronics.design), I would not have much confidence in any results that rely on rDS(on) or device capacitance. I know (by reputation) some of the guys that were posting in that thread. They are truly experts, and they were getting results which did not match the datasheet.
What are you using the part for?
I think I'll change to a different mosfet, then. One that has a tried and true spice model. I actually did get in touch with the guy who resized the model in that google forum. He explained a few things to me about the spice netlist vs. the model card and referencing channel parameters, etc.

I'm just using this fet to sink a cap to ground at regular intervals. Part of a peak detector circuit. Pretty much any old fet will do as long as it switches really fast and doesn't have a great deal of drain-source resistance and capacitance.
 
Status
Not open for further replies.

Latest threads

EE World Online Articles

Loading
Top