Hello,
I tried running a DC operating point simulation of an FQP27P06 P-channel MOSFET in a test circuit (project file attached), using the attached Spice model file, but got no output and no execution listing. Is my pin number mapping between the symbol and the model correct?
Thank you.
FQP27P06 (2).zip (966.3 KB)
Line 9 of file FQP27P06.lib now is
.MODEL DMOS PMOS (VTO=(.00298*TEMP-3.174) KP=-0.0068*TEMP+10.4
Change it to
.MODEL DMOS PMOS (VTO=(.00298*TEMP-3.174) KP=(-0.0068*TEMP+10.4)
EDIT: removed parenthesis, thanks, WilderPumpking76.
Acording to your image it is not correct:
You can check out the library code which indicates the pin connections:
* D G S
.SUBCKT FQP27P06 20 10 30
Drain - 20, Gate - 10, Source - 30.
Thanks @holger, just need one less parentheses there is an additional line of parameters:
.MODEL DMOS PMOS (VTO=(.00298*TEMP-3.174) KP=(-0.0068*TEMP+10.4)
+ THETA=0.0576 VMAX=3.0E5 ETA=0.004 LEVEL=3)
Thank you for indicating the need for parentheses in the KP parameter statement, and for alerting me to a symbol-model mapping issue. I have added the parentheses, but as expected, the simulation still does not run as my pin mapping currently stands.
I’m still not clear on the how the mapping should be done however. There are actually two areas of uncertainty for me.
First, I should mention that I added the *…D G S…" comment to the model file (it was not there originally) in order to guide me as to how the numerics 20, 10 and 30 should refer to the respective MOSFET terminals. This was an educated guess on my part, by noting that the “Rd 20 4 0.018 TC=0.0055” statement apparently refers to a drain parameter, and I associated the included numeric of 20 with that. Similarly, I inferred from “Rg 10 1 1.48” that 10 refers to a gate parameter. This left 30 for the source.
The second area of uncertainty is that I when I assigned the actual mapping, I chose to connect the symbol pin functionality indicated as (G, (D), or (S) on the left side with the Spice model numerics in parentheses on the right side, e.g. (10), (20), and (30) respectively, ignoring the numbers NOT in parentheses - 1, 2, 3, vs. 2, 1, 3. I could be in error in either or both of these procedural steps.
I hope this clarifies what I tried to do and helps me learn the correct methodology. I look forward to being corrected on this and understanding my error. Thanks again.
Please specify: what is the outcome of the op simulation?
For me it seems to be o.k. after adding the parenthesis.
Your ‘educated guess’ is correct. Finally one could check line 8 of the model file:
M1 2 1 3 3 DMOS L=1u W=1u
which is a call to a MOS transistor in ngspice. Its pin sequence is fixed by the simulator, to be
Drain, Gate, Source, Bulk,
with Source and Bulk typically tied together in a 3-pin power device.
After creating a New Analysis tab for the DC operating point, I click on the blue arrow. The two probe buttons on the toolbar flicker momentarily, but going back to the console shows no voltages or currents listed. I tried a couple of things:
- I switched the pin mapping around (using the numbers not in parentheses this time), the simulation again did not run with no printout or errors listed, so this issue may not be related to my pin mapping error.
- I went back to another test circuit (for a 2N2222). This one simulated correctly with no errors.
- I tried the FQP27P06 test circuit again, this time the simulation worked. I noted that this time the two probe buttons changed state properly after clicking on the blue arrow (no flicker).
- I closed this project and reopened it to verify, unfortunately the simulation again did not run, same behavior as the original problem.
I’ll trying switching between the two transistor circuits again to see if there is a pattern.
My circuit now works with the parentheses you specified. I had first tried that change in the model file within the project that I sent to you, but the file path within that uploaded project was not correct. Everything looks good now, thank you.
1 Like