May 5, 2023 at 2:32 pmAdrienSubscriber
I built a modal analysis in ANSYS workbench with an APDL command inside the Solution branch that runs a harmonic analysis, so the harmonic files (rst, mode, full, etc..) are written inside the modal analysis directory.
To separate files generated by both analysis (modal and harmonic), I want to name files generated by the harmonic apdl command with something different than the actuel jobname of the modal analysis (the default name is "file", so for example i want to rename as "fileh", h for "harmonic").
Here is my APDL command (which is inside the "Solution" branch of my modal analysis) :
RESUME ! load the .db file
/com,*********** Defining Loadings ***********
/com,*********** Create Base Excitation**********
_loadvari6528z(1,1,1) = magnitude
_loadvari6528zi(1,1,1) = phase
ANTYPE, MODAL, RESTART ! restarting the modal analysis
MODCONT, ON, ON ! enforced motion turned on
/COM,*********** Defining Base Excitation ***********
[Selection of my base excitation]
/com,*********** Performing MSUP Harmonic Solve ***********
HROPT, MSUP, , , YES ! I want to get the mcf file of the harmonic analysis
[Settings for my harmonic analysis]
/com,*********** Applying Base Excitation(s) ***********
I don't know where to put my "FILNAME" command, because if I put it on the session level, it says "fileh.mode and fileh.full doesn't exist", as if "fileh" was my modal analysis jobname...
Do you have any idea of how changing the harmonic files names ?
May 8, 2023 at 12:39 pmChandra SekaranAnsys Employee
From this input it looks like the modal analysis is already done. You are doing a restart of the modal analysis to create load vectors. Did you do the modal analysis in this same directory? The modal restart as well as the mode sup harmonic requires files from your modal analysis. I would just copy all the files from the original modal analysis to the directory where you are running the harmonic analysis. In this case there is no need to change the jobname.
May 9, 2023 at 6:55 amAdrienSubscriber
Thank you for your reply.
Indeed, my modal analysis is already done before the execution of the APDL command, because the APDL command is in the “Solution” branch. I’m doing a restart of the modal analysis to create load vectors, yes. I did the modal analysis in the same directory, yes : in the default directory of the modal analysis, and I want to make the harmonic analysis in the same directory.
I want to avoid copying files because that’s the reason why the harmonic analysis make so much time to perform (i guess, maybe i’m mistaking ?) – the rst and mode files are pretty heavy. So i want ansys to write directly the harmonic files in the same directory as the modal one. In reality, it works but the harmonic files overwrite the modal files in this directory (rst, mode, full, out), so every time I want to re-perform the harmonic analysis (for any reason like changing some analysis parameters), I have to perform both modal and harmonic analyses (because ANSYS can not find the .rst, .mode and .full files of the modal analysis to perform the harmonic because they correspond to the previous harmonic files), which can take unnecessary time. I want to avoid that and treat hamonic analysis separatly from the modal one.
May 9, 2023 at 11:52 amChandra SekaranAnsys Employee
To avoid copying the modal analysis files you can use the MODDIR command to point to the modal files . A typical sequence is shown below. This way you can run your harmonic analysis in a different directory but use the files from the modal anlaysis without copying them over.
antype,modal,restart ! restarting the modal analysis
thexpand,off ! ignore thermal strains
mxpand,,,,yes,,no, ! expand element results, but not write them to file.mode
- You must be logged in to reply to this topic.
Boost Ansys Fluent Simulations with AWS
Computational Fluid Dynamics (CFD) helps engineers design products in which the flow of fluid components is a significant challenge. These different use cases often require large complex models to solve on a traditional workstation. Click here to join this event to learn how to leverage Ansys Fluids on the cloud, thanks to Ansys Gateway powered by AWS.
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.
- Solver Pivot Warning in Beam Element Model
- Saving & sharing of Working project files in .wbpz format
- Understanding Force Convergence Solution Output
- An Unknown error occurred during solution. Check the Solver Output…..
- What is the difference between bonded contact region and fixed joint
- User manual
- The solver engine was unable to converge on a solution for the nonlinear problem as constrained.
- whether have the difference between using contact and target bodies
- material damping and modal analysis
- Colors and Mesh Display
© 2023 Copyright ANSYS, Inc. All rights reserved.