@Talha Bin Azmat is it ok to add .va file using edit attributes of reram? Is that how you have simulated reram circuit?

@Binoy B I have yet to test this myself, but see this: https://github.com/barakhoffer/sky130_xyce_reram

@Stefan Schippers Do I have to modify the sky130.lib.spice to include spice model for reram? How is it done?

@Talha Bin Azmat how have you done the installtion of xyce ? I have difficulty in installing Trilinos. Any help?

Has anyone been able to successfully extract reram devices in magic for LVS purposes? I'm on magic 8.3.315 and magic treats the device as a via so TE and BE are shorted. Maybe this is a pdk version issue?

hi , did anybody calculate the Ron / Roff from the veriloga model supplied ?

Hi All, Does SKYwater RRAM model have a variability model?

Hi all, I added an install script for this in the repo. Also, I created an example using colab, that also shows how to install spack and compile xyce via spack (and backup the binaries in google drive): https://colab.research.google.com/github/barakhoffer/sky130_xyce_reram/blob/main/Sky130_ReRAM_Xyce.ipynb 😀

@Matt Venn has left the channel

I have seen that ngspice has very recently switched from ADMS to OSDI (OpenVAF) verilog-A support. This allows to easily build verilog-A models (example: reram) and simulate without doing magic things like rebuilding ngspice. Has anyone had a chance to look at this? in the coming days I want to update the xschem reram model according to this change.(cc @Talha Bin Azmat @Tim Edwards) If someone has already done some investigation please let me know. I have already built ngspice-39 and downloaded the openvaf compiler so i am ready to go...

@Barak Hoffer I have updated the tb_reram.sch test circuit (and the reram.sym component) in xschem_sky130 to use the new OSDI/OpenVAF interface with ngspice. If I increase the voltage source to

2V

peak value I see some current bump. I don't know if this is correct, but at least something is happening. May be reram parameters must be tuned somehow... WIll also try to compare with Xyce, if I am able to do that...

The schematic looks good! I also see the peek at 2V, but there is not state change as needed when going back to lower voltages.

@Stefan Schippers: What would I need to do to add the OpenVAF model to the PDK so that it is available when doing an open_pdks build?

Hi, @Tim Edwards what I did was to clone this reram repo, then use the

openvaf

compiler (openvaf is a prebuilt executable I downloaded from the openvaf main site). Then simply compiled the

sky130_fd_pr_reram_git/cells/reram_cell/sky130_fd_pr_reram__reram_cell.va

to produce the

sky130_fd_pr_reram__reram_cell.osdi

object. This must be included in ngspice with the new

pre_osd

command. Following is the complete netlist of the testbench:

** sch_path: /home/schippes/.xschem/xschem_library/xschem_sky130/sky130_tests/tb_reram.sch
**.subckt tb_reram
N1 TOP 0 sky130_fd_pr_reram__reram_model
V1 TOP 0 PWL (0 0 1u 2 2u 0 3u -2 4.0u 0.0)
**** begin user architecture code
.control
  * Modify according to your specific location
  pre_osdi /mnt/sda7/sky130_fd_pr_reram_git/cells/reram_cell/sky130_fd_pr_reram__reram_cell.osdi
  save all
  tran 1n 4.0u
  write tb_reram.raw
.endc
** opencircuitdesign pdks install, not needed in this testbench
* .lib /home/schippes/share/pdk/sky130A/libs.tech/ngspice/sky130.lib.spice tt
**.ends

.model sky130_fd_pr_reram__reram_model sky130_fd_pr_reram__reram_cell area_ox=0.1024e-12  Tox=5.0e-9
+  Tfilament_max=4.9e-9  Tfilament_min=3.3e-9  Tfilament_0=3.5e-9  Eact_generation=1.501  Eact_recombination=1.500
+  I_k1=6.140e-5  Tfilament_ref=4.7249e-9  V_ref=0.430  velocity_k1=150  gamma_k0=16.5  gamma_k1=-1.25
+   Temperature_0=300  C_thermal=3.1825e-16  tau_thermal=0.23e-9  t_step=1.0e-9

**** end user architecture code
.end

You see the reram instance uses the (new)

N

letter, it references a

sky130_fd_pr_reram__reram_model

SPICE model, this can be defined as simply

.model sky130_fd_pr_reram__reram_model sky130_fd_pr_reram__reram_cell

the

.model

'*connects*' the spice device to the verilog OSDI model Additionally the .model can override default parameters specified in the .va file, as done in above netlist . To enable the new reram I think the

.model sky130_fd_pr_reram__reram_model

SPICE wrapper and the

<http://sky130_fd_pr_reram__reram_cell.va|sky130_fd_pr_reram__reram_cell.va>

verilog source file should be added. Then the verilog must be compiled on the target machine in some way.

Check out my repo for the reram model using openvaf and ngspice: https://github.com/barakhoffer/sky130_ngspice_reram I have updated the model and turned it to a well-posed one and now it shows switching of the ReRAM device when simulating with ngspice!

Did people here see https://twitter.com/maxhodak_/status/1635330756276015105 (and https://science.xyz/services/foundry )?

Hello, I attempted to utilize the reram model with the pre_osdi command, but ngspice displayed an error stating that it could not recognize the osdi command, despite using ngspice-39. Could you please explain why this is happening? @Stefan Schippers

Hi All, I am completely new to circuit design, and we started using the sky130 process for our design since it has the option for a mix-signal design using a reram cell. I installed xschem, magic and open-pdk an ngspice-38 using ADMS. However, when i tried to simulate the I-V output for the reram cell i got the following error on ngspice: The first issue: % l_s_d(): Symbol not found: /home/schippes/share/xschem/xschem_library/devices/vsource.sym l_s_d(): Symbol not found: /home/schippes/share/xschem/xschem_library/devices/vsource.sym However, the library for the reram is installed with other sky130 libraries in my local directory not the path given in the error message.when I press on the current/voltage source and edit the path for vsource to be my local directory for vsource I got the following error: Circuit: ** sch_path: /home/eda_work/eman/hassan/open_pdks/sources/xschem_sky130/sky130_tests/tb_reram.sch Error on line 3 or its substitute: n1 top 0 sky130_fd_pr_reram__reram_model unknown device type - error The simulation interrupted due to an error!. I am not sure what is the problem and how i can fix it. Appreciate your help in this regard. Note : I installed the open_pdk, sxchem and ngspice using the following video instructions: @Stefan Schippers YouTube | Stefan Schippers

Install xschem + xschem_sky130 + skywater-pdk + ngspice on your linux system▾

Thank you for the response. However, the instructions you added to Jupyter could be clearer to me. Sorry, I am still learning, and I am a bit confused.

now i got the following error when using ngspice to test the reram model available in xschem : Note: No compatibility mode selected! Error opening osdi lib "/mnt/sda7/sky130_fd_pr_reram_git/cells/reram_cell/sky130_fd_pr_reram__reram_cell.osdi": No such file or directory! Error: Library /mnt/sda7/sky130_fd_pr_reram_git/cells/reram_cell/sky130_fd_pr_reram__reram_cell.osdi couldn't be loaded! Circuit: ** sch_path: /home/eman/.xschem/xschem_library/xschem_sky130/sky130_tests/tb_reram.sch Error: unknown subckt: x2 3v Simulation interrupted due to error! Hpwever, when I follow the steps ngspice 1 -> However, when I follow the steps in repo:https://github.com/barakhoffer/sky130_ngspice_reram to plot the I-V for reram I got the following plo, which does not reflect the reram behavior

Screen Shot 2023-04-12 at 6.17.53 PM.png

Looks good! I would just change it and take the negative of the voltage source current so it will be clearer

Hi All, after i tried to fix the above error, I end up with the following error when tried to simulate the rearm cell. Error on line 5 or its substitute: n1 top 0 sky130_fd_pr_reram__reram_model could not find a valid modelname Simulation interrupted due to error!. why it cant recognize the reram model?

On the other side, we are using cadence tools with spector simulator for our circuit analysis. Is there a compatible spice model that we can use for virtuoso and spector?

Hi All, after update/reinstall the open_pdk, and when try to simulate the reram_tb using ngspice I got the following errors: Note: Compatibility modes selected: hs a Error opening osdi lib "/home/eda_work/eman/hassan/share/pdk/sky130b/libs.tech/ngspice/sky130_fd_pr_reram__reram_module.osdi": No such file or directory! Error: Library /home/eda_work/eman/hassan/share/pdk/sky130b/libs.tech/ngspice/sky130_fd_pr_reram__reram_module.osdi couldn't be loaded! Circuit: ** sch_path: /home/eda_work/eman/hassan/share/pdk/sky130b/libs.tech/xschem/sky130_tests/tb_reram.sch Error on line: n.xr1.n1 top 0 xr1.nfilament sky130_fd_pr_reram__reram_model could not find a valid modelname Simulation interrupted due to error! any advice? @Stefan Schippers @Barak Hoffer @mkk @Tim Edwards

Hi All, thank you @Stefan Schippers for your prompt response: I have already clone the https://github.com/barakhoffer/sky130_ngspice_reram (@Barak Hoffer) and I have

<http://sky130_fd_pr_reram__reram_module.va|sky130_fd_pr_reram__reram_module.va>

sky130_fd_pr_reram__reram_module.osdi

in the path /home/eda_work/eman/hassan/share/pdk/sky130B/libs.tech/ngspice. the current PDK_ROOT I added to the .bashrc are

export PDK_ROOT=/home/eda_work/eman/hassan/share/pdk

when i checked the netlist for tb_reram test case I got the following:

** sch_path: /home/eda_work/eman/hassan/share/pdk/sky130B/libs.tech/xschem/sky130_tests/tb_reram.sch

**.subckt tb_reram

V1 net1 0 PWL (0 0 0.25u 1.8 0.5u 0 0.75u -1.8 1.0u 0.0)

.save i(v1)

XR1 TOP 0 sky130_fd_pr_reram__reram_cell Tfilament_0=3.8e-9

Vreram net1 TOP 0

.save i(vreram)

**** begin user architecture code

.control

save all

tran 0.1n 1.5u

write tb_reram.raw

.endc

**** end user architecture code

**.ends

**** begin user architecture code

.subckt sky130_fd_pr_reram__reram_cell TE BE Tfilament_0=3.3e-9 area_ox=0.1024e-12

N1 TE BE nFilament sky130_fd_pr_reram__reram_model

.ic v(nFilament)={Tfilament_0*1.0e9}

.ends sky130_fd_pr_reram__reram_cell

.model sky130_fd_pr_reram__reram_model sky130_fd_pr_reram__reram_module area_ox=0.1024e-12  area_ox

+ = 0.1024e-12  Tox = 5.0  Tfilament_max = 4.9  Tfilament_min = 3.3  Eact_generation = 1.501

+  Eact_recombination  = 1.500  I_k1  = 6.140e-5  Tfilament_ref = 4.7249  V_ref = 0.430  velocity_k1 = 150  gamma_k0  =

+ 16.5  gamma_k1  = -1.25  Temperature_0 = 300  C_thermal = 3.1825e-16  tau_thermal = 0.23e-9  t_step  =

+ 1.0e-9  smoothing = 1e-7  Kclip = 200

.control

pre_osdi

+ /home/eda_work/eman/hassan/share/pdk/sky130B/libs.tech/ngspice/sky130_fd_pr_reram__reram_module.osdi

.endc

How many cycles can a SKY130 ReRAM cell survive? Just curious about the feasability of implementing the HH model using the memristor analogy.

Hi All, Any advice about the previous question in the following thread? https://open-source-silicon.slack.com/archives/C02Q2DE33QF/p1681642289780979

Hi All, thank you, @Stefan Schippers for your response. I mean after cloning the https://github.com/barakhoffer/sky130_ngspice_reram and having the

<http://sky130_fd_pr_reram__reram_module.va|sky130_fd_pr_reram__reram_module.va>

sky130_fd_pr_reram__reram_module.osdi

in the pdk path in the path /home/eda_work/eman/hassan/share/pdk/sky130B/libs.tech/ngspice. Also, the current PKK_ROOT is: export PDK_ROOT=/home/eda_work/eman/hassan/share/pdk. However, I have still has the same error when I tried to simulate the tb_reram available in the path

sch_path: /home/eda_work/eman/hassan/share/pdk/sky130B/libs.tech/xschem/sky130_tests/tb_reram.sch

the error is as the following: Error opening osdi lib "/home/eda_work/eman/hassan/share/pdk/sky130b/libs.tech/ngspice/sky130_fd_pr_reram__reram_module.osdi": No such file or directory! Error: Library /home/eda_work/eman/hassan/share/pdk/sky130b/libs.tech/ngspice/sky130_fd_pr_reram__reram_module.osdi couldn't be loaded! Circuit: ** sch_path: /home/eda_work/eman/hassan/share/pdk/sky130b/libs.tech/xschem/sky130_tests/tb_reram.sch Error on line: n.xr1.n1 top 0 xr1.nfilament sky130_fd_pr_reram__reram_model could not find a valid modelname Simulation interrupted due to error!. I am not sure what I missed and how to fix the issue.