Someone could help me in making these pspice models more pleasant to qspice?
Many thanks guys
RHR801_pspice_beginning_of_life_rev1.txt (9.4 KB)
TS3011.txt (17.9 KB)
Could you explain further what exactly you are looking for?
When importing pspice model into qspice, I often get warning messages in the “Output Window”, followed by failures finding an operating point and finally by a fatal error (i.e. timestep too small).
This is what I get specifically with the attached models.
Are most of these warning messages due to a syntax incompatibility between programs? Honestly I wouldn’t know.
In other cases of importing models from third parties, moreover, it happens that apparently only very slow simulations can be performed.
Many thx for your support
Upload your example for review.
RHR801_QSPICE.qsch (10.1 KB)
Try this for example.
It seems that going directly to Gmin stepping and playing with gshunt, something happens for some values but warnings persist.
I’m not sure all can be ignored.
Tweaking models is not my area of expertise. Since this is a high-speed comparator, I focused on running the model at the MHz level. I have added my comments to the schematic.
The major tweak to help with transient convergence for this model was adding CJO=2p to the diode model. Sometimes, smoothing the diode transition with CJO can help improve convergence during switching.
RHR801_QSPICE.qsch (5.1 KB)
RHR801_pspice_beginning_of_life_rev1-Qspice.txt (9.5 KB)
However, if you are planning a more complicated project, depending on the level of detail you would like to include, replacing it with an HMITT with proper delay, rise, and fall time matching might be a more robust simulation choice. There is also no guarantee regarding the quality of the models provided by manufacturers. In general, a simulation task only requires the inclusion of critical behaviors.
RHR801_QSPICE-HMITT.qsch (6.9 KB)
Thanks for your time! Available to lend a hand as always.
Obviously I had already modelled the basic characteristics of the component with a SCHMITT port for preliminary tests on the simulator.
And for sure, the final check at the workbench is always due.
That’s why it’s often reported a remark like “Macromodels are not a substitute to bread-boarding” within the MFR files.
But in cases where (as for RHR801) electronic components have a significant cost, or have a significant procurement time, it is important from the first steps to use a simulation model that is as faithful to reality as possible.
I think that the qspice’s poor compatibility with many of the simulation models provided by manufacturers is a significant bottleneck for the widespread use of this nice simulation tool.
But an online database shared and verified by a community could be of great help.
Understand. Compatibility keeps improving based on my experience; at least, there are fewer complaints regarding TI PSpice models as from forum. Of course, QSpice cannot run LTspice models that use A-devices, as those are IP-restricted. But with more people use Qspice and reporting issues, compatibility will keep improving.
In general, which manufacturer(s) provide models that you think currently have poor compatibility with QSpice?
Here is a more robust tweak. Replacing .SUBCKT VCCAP_PSPICE with Arbitrary Capacitance-Based model (one line Qspice syntax instead of multiples line Pspice version). This is where the major area Qspice fails to convergence for DC solution, which is a voltage controlled capacitor model. Reduce CJO to 1f to minimizing diode capacitance but reserve a bit help in transient convergence. I didn’t add that to TS3011 as the example run fine without that 1pF. So far they run with Qspice64.exe or Qspice80.exe.
example.RHR801.qsch (4.8 KB)
RHR801_pspice_beginning_of_life_rev1-Qspice-VCCAP_PSPICE.txt (9.6 KB)
example.TS3011.qsch (4.8 KB)
TS3011-Qspice-VCCAP_PSPICE.txt (9.3 KB)
Here is verification of equivalent circuit for .SUBCKT VCCAP_PSPICE
equivalent.VCCAP_PSPICE.qsch (12.9 KB)
I generally use ICs from TI, ST, AD/LT, Intersil/RENESAS, Skyworks, …
Do you know if there is already a shared database of third parties components whose simulation models have already been analyzed and verified through the forum?