May 19, 2021 at 8:48 amfloatingstonesSubscriber
I am doing a load mapping from Aqwa to Mechanical. The following warning appears when I try to generate a Hydrodynamic Pressure in Mechanical:May 19, 2021 at 11:53 amErik KostsonAnsys EmployeeHi
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
May 19, 2021 at 1:02 pmMike PettitAnsys 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.
May 20, 2021 at 9:30 amfloatingstonesSubscriberIt was exactly that thank you again for your help!
May 25, 2021 at 9:22 amfloatingstonesSubscriber-
May 25, 2021 at 10:48 amMike PettitAnsys 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.
May 27, 2021 at 1:22 pmfloatingstonesSubscriber!
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...
May 27, 2021 at 1:39 pmMike PettitAnsys 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.)
June 8, 2021 at 11:39 amfloatingstonesSubscriber. Thank you! This is a great tip, I'll be sure to use it if I ever need it :)
June 24, 2021 at 3:32 pmetquistSubscriber. 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!
June 24, 2021 at 3:44 pmMike PettitAnsys 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.
June 24, 2021 at 3:48 pmetquistSubscriber
Oh okay, thank you for the quick response!
Viewing 11 reply threads
Ansys Innovation Space
- You must be logged in to reply to this topic.
Simulation World 2022
Check out more than 70 different sessions now available on demand. Get inspired as you hear from visionary companies, leading researchers and educators from around the globe on a variety of topics from life-saving improvements in healthcare, to bold new realities of space travel. Take a leap of certainty and check out a session today here.
Earth Rescue – An Ansys Online Series
The climate crisis is here. But so is the human ingenuity to fight it. Earth Rescue reveals what visionary companies are doing today to engineer radical new ideas in the fight against climate change. Click here to watch the first episode.
Subscribe to the Ansys Blog to get great new content about the power of simulation delivered right to your email on a weekly basis. With content from Ansys experts, partners and customers you will learn about product development advances, thought leadership and trends and tips to better use Ansys tools. Sign up here.Trending discussions
- How to calculate the residual stress on a coating by Vickers indentation?
- An Unknown error occurred during solution. Check the Solver Output…..
- Saving & sharing of Working project files in .wbpz format
- Solver Pivot Warning in Beam Element Model
- Understanding Force Convergence Solution Output
- Colors and Mesh Display
- whether have the difference between using contact and target bodies
- The solver engine was unable to converge on a solution for the nonlinear problem as constrained.
- What is the difference between bonded contact region and fixed joint
- Massive amount of memory (RAM) required for solve
Top Rated Tags
© 2022 Copyright ANSYS, Inc. All rights reserved.Ansys does not support the usage of unauthorized Ansys software. Please visit www.ansys.com to obtain an official distribution.