September 21, 2023 at 5:49 pmLouie LouSubscriber
I try to do aircraft wing fatigue life analysis. I have acceleration-time data (1G-1.5G) more than 20000 datas. I determined boundary conditions for wing (acceleration). I converted acceleration-time graph to PSD to add fatigue tool history data. However, I have a problem. How can I calculate the life cycle as hours and infinite life? How can I use the Rainflow Cycle to calculate it?
September 22, 2023 at 2:26 pmAshish KhemkaForum Moderator
Please see if the following link is of help to you:
Thanks and Regards,
September 22, 2023 at 3:46 pmLouie LouSubscriber
Thank you for answer, however I have a different problem. I have almost 98700 acceleration datas for aircraft's wing. I will pit them the history data to calculate fatigue life. I want to find 1 block is how many hours? How can I calculate it?
September 23, 2023 at 3:40 amLouie LouSubscriber
I want to give detail. It is going to more than 2000 datas.
I have 2 questions.
1- How can I find the 1 cycle/block is equal to how many hours?
2- Should I convert acceleration-time to PSD to put history data or must I put as acceleration-time?
time acceleation 0.1 9,80 0.2 10,7 0.3 9,8 0.4 9,8 0.5 9,79 0.6 10,8 0.7 9,8 … ...
September 27, 2023 at 6:46 amAshish KhemkaForum Moderator
Thanks for the update. I do have an answer to this query. Please wait for other members to comment.
September 28, 2023 at 4:16 amDaniel ShawAnsys Employee
I assume that you are using the Mechanical Fatigue Tool (FT) with time history loading (non-constant amplitude, proportional loading). If so, the FT outputs life in repeats of the loading cycle. For example, if your loading cycle represents 1 hour of operation then reported life is repeats of 1 hour of operation.
The FT internally uses rainflow counting to organize the stresses into “bins or blocks” of data that represent stress ranges and mean stresses. You can block the rainflow matrix, but the FT will not report the fatigue damage per bin.
If you have the time history loading, you should not need to use a random vibration approach.
September 28, 2023 at 4:28 amLouie LouSubscriber
Thank you so much sir. I have changed the fatigue analysis program as nCode DesignLife.
You said ''If you have the time history loading, you should not need to use a random vibration approach'' I thought Since I use nCode, I need to transfer this acceleration-time data to the system. So I thought of doing an analysis using vibration generator. Am I right?
Static Structural - nCode DesignLife (Time Series SN) - Excel Input - Vibration Generator - Analysis - Result
Is it true or not? In addition, should I add acceleration condition on model in static structural? I have moment condition too. I know the fatigue, however I can't realize the thought in my head. I need your help sir.
September 28, 2023 at 1:38 pmDaniel ShawAnsys Employee
Are the data in the acceleration table multipliers on the applied acceleration in the FE model? If so, why can’t you use a Time Series Load Mapper in Ansys nCode DesignLife? DesignLife time series load mapping uses one set of FE results and scale factors from a time history file to create time varying stress. If you can convert your time base acceleration data to a PSD spectrum, you can run a DesignLife vibration fatigue analysis using that spectrum, but I do not see why it is necessary (or preferred).
Is the moment load constant or does it vary with time? If it is a constant load, then the stress it produces does not directly contribute to the alternating stress. It acts a mean stress. The DesignLife time series load mapper has an option to specify a “static” result set. The stresses from the static result set will not vary over time, but they will be used in any mean stress calculations.
September 28, 2023 at 3:28 pmLouie LouSubscriber
My acceleration-time datas are in Excel table. There is acceleration(1G) condition in FE Model. My datas must effect my wing acceleration from 1g to 1.5g with time, and I want to see after 2000 sec, my fatigue life in FE Model
There is moment which is constant in FE model.
I want to analyze that performing fatigue analysis of my wing, whose acceleration changes during the flight between 1-1.5g.
What should my workflow be?
September 28, 2023 at 3:38 pmLouie LouSubscriber
In addition you are right vibration analysis is not necessary, but I want to add acceleration-time datas on acceleration which is in FE Model. I hope I explained my problem
September 28, 2023 at 6:39 pmDaniel ShawAnsys Employee
Walking you through a complete Ansys nCode DesignLife fatigue analysis is beyond the scope of this forum. I can only provide some guidance. In addition, there are multiple acceptable approaches. I cannot know the best approach without obtaining more details. I recommend searching AIS for the “Introduction to Ansys nCode DesignLife “training course. That training course will explain how to set up an Ansys nCode DesignLife time series analysis. I also recommend reviewing the first 2 Worked Examples in the Ansys DesignLife Help (see below).
If you are using 22R1 or later, I recommend using the Ansys nCode DesignLife Mechanical Add-On (WE#1). If you are using an early release, I recommend using the Ansys nCode DesignLife Workbench Integrated systems (WE#2). You can also use the HBK standalone Glyphworks interface, but I do believe that approach is required and it requires more DesignLife knowledge.
A quick summary of the required steps.
1. Run Mechanical model with 2 load steps: static moment and unit acceleration
2. Store the acceleration load multipliers as a single column time history file in the appropriate format (ASCII for embedded Add-On and .s3t for the Integrated systems)
3. Choose the appropriate set-up for a time-series analysis (depends on the interface)
4. Choose time-series load mapper and read in Mechanical result sets
5. Set the moment result in the load mapper to be “static”
6. Associate the acceleration load step in the load mapper with the time history file.
7. Specify the appropriate mean stress method
October 1, 2023 at 9:46 amLouie LouSubscriber
I searhed many times, however I cannot add my excel datas(acceleration-time) in nCode DesignLife. How can I convert excel data to s3t? Time series input does not see excel datas on workspace
EDIT : I solved the problem
October 2, 2023 at 7:11 amLouie LouSubscriber
I hope you are good today :)
We have talked before about calculating from life cycle to hours. I confused a bit. You know I have acceleration-time data and time finishes at 9700 second. I analyzed my model life which is 389000 cycles, so should I (9700x389000)/(3600) to calculate as hours life?
September 28, 2023 at 7:02 pmLouie LouSubscriber
Sir, you are the best. Thank you so much :) I'll do it and I'll watch every video.
- 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.
- How to do the frequency response of the nonlinear vibration of a flexible PCB?
- Importing Line and Solid Bodies from SpaceClaim to Mechanical
- how to open SendCommand in Ansys
- problems facing during solution
- Still facing the same issue
- Failed to move file from solver directory to scratch directory: file.rst
- Adaptive Sizing
- Stiffness factor
- Import DAT file
- Import pressure data (coordinates and value) to ansys workbench through excel
© 2023 Copyright ANSYS, Inc. All rights reserved.