Stats

More Content

Module 1: Simulation produces error: Mass is not a number

SimonGohle

The problem I have with the first challenge might be a problem with my PC. When ever I start the simulation of the in the handout specified numbers, the simulation ends after some time and gives out the error message

 - S_Simulation 1 Error: ERROR: residual of Mass is Not A Number: the solver has been stopped

and the message

 - The simulation Simulation 1 has failed: some NaN have been detected during the computation.<br> ERROR: residual of Mass is Not A Number: the solver has been stopped

I don´t know if my PC´s CPU is maybe not good enough or if there might be a problem with my pre-processing in this challenge.

What worked is to set the CFL Number to 1.5 instead of 3.0, but the challenge requires running the simulation with a CFL of 3.0.

Parents
  • 0
    Hi Simon,

    I assume you are using Omnis v5.2? Good news is: this problem does not originate from your CPU! This is what we call a diverging/crashing simulation. You did the proof yourself: By setting CFL to 1 the simulation does not converge anymore. Please try the following: Set the CFL to 3 and the CFL number (for CGI) to 1 as shown in the screenshot below.
    IF you are in essential mode, you just see the CFL number, which shall be put to 3. We were assuming that you would remain in essential mode.

    Could you please check if that solves the problem and give us a quick feedback? If that helps we would quickly update the hand-out.

    Best regards,
    Kathrin
  • 0 in reply to Kathrin

    Yes, I am using Omnis v5.2 . It is the other way around, if I set the CFL number on 3.0 it will produce the error, but if I set it on 1.5 it works. I looked into the program and CFL number is at 3 and CFL number (for CGI) is already at 1. I tried it also with lower speeds of 0.5 m/s, and then it worked fine with a CFL number of 3. So that is unfortunately not the solution I am searching

  • 0 in reply to Kathrin

    Yes, I have laminar Flow on and a tip at Low speeds with the correct velocity when the Error is produced.

  • +1 in reply to SimonGohle

    I found my error. There is a tab in the mesharea exactly looking the same for the viscos layers. Instead of setting it up in at the wall I set it up in the mesh set up in the tab local. That producet the error. Now my Solution converges. Thank you very much for your help :)

  • 0 in reply to SimonGohle

    hi together,

    I have the same issue like you Simon, but I can’t  follow your way of fixing it. I only found the tab from Kathrins screenshot at "simulation"    --> "domain" --> "physics" but there is everything correct.

    I also checked the CFL Number part but I have the same settings like you.

    Best regards,

    Lukas

  • +1 in reply to LukasOde

    Hi Lukas,

    to my understaning Simon has set up viscous layers not only on the walls but also on inlet and outlet because he used the "local" tab in the mehs setup.

    Please try the following:

    • Select the mesh setup: Make sure that full hexa mesh and a cell size in domain of 0.0025m has been set.
    • Select the mesh setup: Go to the tab local: make sure that viscous layers is deactivated there. The box needs to been unticked. Otherwise the visous layers are inserted on the whole grid.
    • Select the boundary of your pipe wall: You are automatically in the tab local. Activate the viscous layers here with the setting from the hand-out: first layer thickness: 9.0e-05 m; target number of layers (fixed): 5

    Viscous layers will be a topic in class 2, but here is already some background: Below you see a cutting plane inside the pipe showing the cell intersection (done in the same way as in result analysis; select cells intersection on the cutting plane and activate the wireframe visibility).

    The upper screen shot shows a grid with visous layers only on the pipe wall. The lower picture shows a grid with viscous layers on wall, inlet and outlet. A simulation with viscous layers on inlet or outlet will diverge in most of the cases with default numerical parameters. So this is already a very good lessons learned: If your simulation diverges/crashes, check that you don't have viscous layers on inlet & outlet.

Reply
  • +1 in reply to LukasOde

    Hi Lukas,

    to my understaning Simon has set up viscous layers not only on the walls but also on inlet and outlet because he used the "local" tab in the mehs setup.

    Please try the following:

    • Select the mesh setup: Make sure that full hexa mesh and a cell size in domain of 0.0025m has been set.
    • Select the mesh setup: Go to the tab local: make sure that viscous layers is deactivated there. The box needs to been unticked. Otherwise the visous layers are inserted on the whole grid.
    • Select the boundary of your pipe wall: You are automatically in the tab local. Activate the viscous layers here with the setting from the hand-out: first layer thickness: 9.0e-05 m; target number of layers (fixed): 5

    Viscous layers will be a topic in class 2, but here is already some background: Below you see a cutting plane inside the pipe showing the cell intersection (done in the same way as in result analysis; select cells intersection on the cutting plane and activate the wireframe visibility).

    The upper screen shot shows a grid with visous layers only on the pipe wall. The lower picture shows a grid with viscous layers on wall, inlet and outlet. A simulation with viscous layers on inlet or outlet will diverge in most of the cases with default numerical parameters. So this is already a very good lessons learned: If your simulation diverges/crashes, check that you don't have viscous layers on inlet & outlet.

Children
Cadence Guidelines

Community Guidelines

The Cadence Design Communities support Cadence users and technologists interacting to exchange ideas, news, technical information, and best practices to solve problems and get the most from Cadence technology. The community is open to everyone, and to provide the most value, we require participants to follow our Community Guidelines that facilitate a quality exchange of ideas and information. By accessing, contributing, using or downloading any materials from the site, you agree to be bound by the full Community Guidelines.