General Mechanical

General Mechanical

Warning: No applicable Aqwa Restart File could be found

    • floatingstones
      Subscriber

      I am doing a load mapping from Aqwa to Mechanical. The following warning appears when I try to generate a Hydrodynamic Pressure in Mechanical:

    • Erik Kostson
      Ansys Employee
      Hi

      I do not have any experience with this, but perhaps some of my colleagues can be of help and provide some feedback (e.g., ).

      All the best

      Erik
    • Mike Pettit
      Ansys Employee

      When you want to do pressure mapping from Aqwa to Mechanical, it is essential that you right-click > Update the Hydrodynamic Diffraction Solution cell (from the Project Schematic) to instigate the hydrodynamic solve (rather than hitting Solve from inside Aqwa Workbench). This is because the Project Schematic application controls the copying of the hydrodynamic files over to the structural directory.
      You should Clear Generated Data in Aqwa Workbench, then Update from the Project Schematic, and then try opening Mechanical again.
      Cheers, Mike
    • floatingstones
      Subscriber
      It was exactly that thank you again for your help!
    • floatingstones
      Subscriber
      -
    • Mike Pettit
      Ansys Employee

      Just to check, are you still trying to map from a Hydrodynamic Diffraction system? (We can also map pressures from a time domain Hydrodynamic Response system with Analysis Type of Irregular Wave Response or Regular Wave Response and with Time Domain Pressure Output options set, but not from Hydrodynamic Response systems with Computation Type of Stability Analysis or Frequency Statistical Analysis, and not from time domain calculations include slow drift effects.)
      When you hit Update on the Project Schematic, was the Mechanical editor open or closed? If it was open, is the problem resolved by closing and re-opening Mechanical? - you may see a message saying 'Upstream data needs to be re-read. Would you like to read the upstream data?' - say Yes to this.
      Cheers, Mike
    • floatingstones
      Subscriber
      !
      Yes, I encountered the same problem when mapping from a HD system. The troubleshooting that you first proposed wasn't working (or I performed it awfully). To be fair, I am not truly sure of what I did when I managed to solve it. I tried to maintain both editors closed when updating, & re-reading upstream data. Hopefully it won't happen again...
    • Mike Pettit
      Ansys Employee

      If you get properly stuck there is always the option to copy the hydrodynamic files manually (but only do this if you really, really need to).
      From the Hydrodynamic Diffraction solver files directory (for example: example_files\dp0\AQW\AQW\AQ\Analysis), copy Analysis.dat, Analysis.pot, Analysis.res, Analysis.uss, Analysis.vac into a Solution folder insider the Static Structural solver files directory (for example: example_files\dp0\SYS\MECH\Solution). Also create an empty file Analysis.hdd in the same location. You should end up with something like:
      Then, the next time you open Mechanical, the Hydrodynamic Pressure object should pick these files up. Naturally you should be very careful if you have multiple Hydrodynamic Diffraction/Static Structural systems that you are copying between the correct systems. (Note this is a workaround when you have accidentally Solved a hydrodynamic system from inside the Aqwa Workbench editor, instead of using Update from the Project Schematic, and the calculation time too long for you to re-solve.)
      Cheers, Mike
    • floatingstones
      Subscriber
      . Thank you! This is a great tip, I'll be sure to use it if I ever need it :)
    • etquist
      Subscriber
      . I wanted to ask a follow up on your earlier comment: "We can also map pressures from a time domain Hydrodynamic Response system with Analysis Type ofIrregular Wave ResponseorRegular Wave Responseand with Time Domain Pressure Output options set".
      I've been working to implement this, but have been consistently receiving this error message:
      My project schematic looks like this:
      I've been able to implement pressure mapping from Hydrodynamic Diffraction, but haven't been able to do so for the time-based Hydrodynamic Response. The Hydrodynamic Response simulation is a floating structure, that has been greatly simplified to simply responding to a regular wave (the mooring lines, current, etc., have been removed for now). As seen in the schematic, there is a Check next to the Hydrodynamic Pressure in the Structural Analysis, however in the Mechanical viewer I am given the error mentioned before. I've also manually copied the "TimeResponse" solution files into the SYS folder, but they aren't recognized until their name is changed to "Analysis", at which point another error is given:
      Any advice concerning these issues would be greatly appreciated!
    • Mike Pettit
      Ansys Employee

      Sorry I should have mentioned that the pressure mapping from time domain hydrodynamic response calculations has only been added at Release 2021 R1. It looks like you're using Release 2019 R2 - when we first offered frequency domain pressure mapping, as a Beta feature - so you will need to upgrade before you can map time domain pressures.
      Note that the time domain pressure calculation in Aqwa was not implemented until 2021 R1, so there's no way you can do this (even manually) in 2019 R2.
      Cheers, Mike
    • etquist
      Subscriber

      Oh okay, thank you for the quick response!
      Ethan
Viewing 11 reply threads
  • You must be logged in to reply to this topic.