RBA300N10EANS3UA02.txt (24.9 KB)
Hi,
I am not able to use the attached model. I am able to use the model in LTspice. How to implement this model in Qspice? When implementing it in Qspice the model does not work.
Does anyone have a solution to it?
This is an encrypted library for LTspice.
Can’t be used in Qspice?
The file you attached may be a Pspice encrypted model, intended for use only in Pspice. Renesas appears to provide both LTspice and Pspice encrypted models for this FET. I believe the library that can be run in LTspice is not exactly the one you uploaded, but rather another one that you can download from their website. Perhaps you could contact a Renesas application engineer to inquire if a Qspice encrypted model can be provided.
RBA300N10EANS3UA02.txt (46.8 KB)
Manufacturer is providing LTspice model. But not able to use in Qspice.
An encrypted model is encrypted by a particular software and can only be used by that software; that’s the purpose of encryption. Therefore, you must use LTspice or contact the supplier to inquire if they are willing to provide a model file that supports Qspice.
Hi @KSKelvin
I simulated the RDS(on) vs ID curve for a GaN HEMT model using the same test conditions specified in the datasheet. However, the simulation results differ significantly from the datasheet values. I’ve attached the model and the resulting waveforms for reference. Could you check if I’m overlooking something and help me figure out the issue?
GS66506T Rdson vs Idrain.qsch (4.7 KB)
@Vikas2 Only simulate up to about 63A if you are trying to match this model with the curve.
The GS66506T datasheet specifies a maximum pulse drain current of 48A for a pulse width of 50 µs and Vgs = 6V. I assume it is unnecessary to consider conditions where the current is unrealistic. Datasheet curve with x axis max at 80A but the curve stopped before that.
GS66506T Rdson vs Idrain (KSK).qsch (4.9 KB)
This model is from a paper developed by its author to compare a level 3 MFG model, and this part is EOL.
https://www.mdpi.com/2079-9292/10/2/130
https://www.infineon.com/part/GS66506T-TR
1 Like
Thank you for the support, @KSKelvin.
I have read the MDPI paper you attached. The author has developed a LEVEL-3 model for a GaN device.
The paper also includes a graph of the energy stored in COSS. Can that also be obtained using simulation?
If you refer to application note, in general Eoss is calculated by firstly obtains Coss vs Vds; and with this to calculate Eoss = 1/2 * Coss(Vds) * Vds. [*Coss depends on Vds]
GS66506T - Ciss Coss Crss Eoss.qsch (10.5 KB)
1 Like
"Thank you, Kelvin. Your knowledge and expertise are really great. I have a question — the datasheet specifies the gate charge, but it does not provide the current value. In that case, what value of current should be taken for simulation?
As, the datasheet specifies drain current = 22.5A.
Id is not that essential… In datasheet, gate charge is tested up to 5nC. In my test circuit template, Igate is to provide gate charge. By Q = I * t, simulates from 0s to 1s, so, at 1s, charge Q = Igate. This represent the value of Igate have to be 5n.
You got this weird curve as you give too much charge to the gate, gate voltage is 100V in your result. It is lucky that this is only a simulation. 
Anyway, set Igate to 5ns you should get the gate charge profile. (** this model doesn’t give you a gate charge profile close to datasheet… but is acceptable I think)
1 Like
Thank you @KSKelvin. I tried, but the gate charge did not match the datasheet.
Anyways, I have a query on uploading a GaN model. I am unable to upload it to Qspice. Does the attached model is only limited to LTspice or any way to upload in Qspice?
The part number is GAN080-650EBE from Nexperia.
Are you referring to these files? Qspice forum not support to upload file with .lib extension. But in general, SPICE library is text file, you just have to change .lib to .txt for upload.
But, I download these two .zip package, reviewed .lib inside, they are both LTspice encrypted model which can only be run in that encrypted platform.
May be you can contact nexperia application engineer to see if can get unencrypted version or Qspice encrypted version.
You will get a better match to the datasheet gate charge curves if you use a current limited voltage source rather than a current limit resistor. The current limit can be done by replacing the resistor R1 with a current source and an ideal diode. I uploaded a schematic that compares the two approaches for a sample FET included with QSPICE. The drain of the FET is either voltage limited or current limited rather than somewhere in between as it is when using a resistor. The current limit provides a constant slope during the plateau while the gate to drain capacitance is charged.
FET gate charge.qsch (198.1 KB)
FET gate charge.pfg (424 Bytes)
2 Likes
I am not aware about that, great remind. By the way, in Qspice, we can config a current source not to source power by adding instance parameter Vsat, and this can eliminate the diode from this setup. Actually, this is also used in the test circuit for gate charge in Qspice MOSFET Model Generator.
FET gate charge (Vsat).qsch (198.4 KB)
While that is similar, it is not quite the same as the ideal diode. The Vsat parameter sets the voltage across the current source at which it saturates at the limit current. For voltages less than Vsat the current is less than the specified limit. The attached schematic adds another circuit using the Vsat parameter and then steps that parameter from 100 mV to 10 V. You can see from the plot of V(d2)-V(d3) that the two drain voltages are not the same during the turn on transition. The difference can be made very small by reducing Vsat from 1 V to 1 mV.
FET gate charge.qsch (202 KB)
FET gate charge Vsat diff.pfg (800 Bytes)
1 Like
Hi @KSKelvin
I am running a circuit in Ltspice. But when I am changing my temp from 25 degrees to above. I am not able to run the circuit.
Could you kindly check what is missing?? The analysis not going beyond 3.5%
@Vikas2 I suspect this error is due to the timestep being too small. I can run this circuit using a trick recommended by Rohm in Qspice. Well, I have two recommendations:
- This is the Qspice forum. We discuss models from other SPICE platforms or compare simulation results, BUT resolving a circuit that runs in another SPICE platform is beyond the scope here, and you should seek help from the support forum of that platform.
- This question is unrelated to the current topic. Please open a new topic for unrelated posts.
Hii @DennisCHI , @KSKelvin
I simulated a gate charge circuit. But the curves are not that practical as the datasheet. Due to this the values of Qgs and Qgd dffers.
Any other method to make it close to the measurement?
Gate charge Diodes.qsch (1.4 MB)