November 4, 2023 at 10:15 pmFayçal ABDOUNFSubscriber
I did a few months ago a Fatigue analysis of a bracket with Ansys Mechanical APDL. I did whole calculation by script launched in apdl. It was very long et took a lot of time.
Now, I'm just want to perfom this same analysis with Ansys workbench.
I've in input a time-history file .dat with forces about X-axis and Y-axis in function of time :
It's my first fatigue analysis in Ansys workbench. I saw that workbench can import time history data but I've no idea how it works. Do I have to run a runflow to retrieve the cycles with the alternating stress and use it as input on workbench or I have to import my .dat file data and workbench will aumatically allocate the forces at the associated times and at the end I will get the life of my part ?
Note : Each time step have a combinations of Fx and Fy as load.
Thank you in advance.
November 6, 2023 at 6:15 pmDaniel ShawAnsys Employee
The Mechanical Fatigue Tool (FT) supports the “History Data” loading type (often referred to as “Time Series loading”). With history data loading, you associate a history data file (ASCII file containing load multipliers – usually vs time) with a Mechanical result set. The FT creates a stress history using he stresses in the FE result set and the multipliers in the history data file. The FT automatically uses rainflow counting to divide the stress history into bins of alternating stress and mean stress.
If you have 2 different load history files that are associated with different FE loadings (e.g. FX and FY), you must run separate FEAs and do separate FT calculations. You can then use Fatigue Combinations to linearly sum the damages (Miner’s rule).
November 6, 2023 at 9:18 pmFayçal ABDOUNFSubscriber
Thank you for your reply.
So what I understand is that no matter the loads were used in the structural analysis, as we are in linear analysis, Workbench will retrieve the stress of whole elements and will use the “history-data” like a factor to calculate the new stress in each elements and that at each point of the history-data file.
And it will determine the damage at each step and with a summation using Milner rule it will give me the life of the part.
But if no matter the loads we use in the first structural simulation, why when I changed it the results are not the same ?
And So what is the “scale factor” under my history data file location in Ansys WB ?
November 6, 2023 at 10:42 pmDaniel ShawAnsys Employee
Your interpretation is basically correct, except the FT does not use element stresses. It uses the average nodal stresses. It calculates the fatigue damage at each node. Even though the FT (and other fatigue software) uses the term “load mapping” when converting discrete FE results into stress histories, the multipliers are applied to the calculated FE stresses.
I am not sure what you mean by “when I changed it the results are not the same”? Changed what? The stresses used by the FT are the FE stresses multiplied by the factors stored in the history data file. The calculated FE stresses are not affected by the history data file. The internal stresses used by the FT are affected. The FT is a post-processing operation.
The scale factor is just another available multiplier. It is a constant multiplier used for all stresses. So, the total FT stress is the FE stress*multiplier from history data file*scale factor. The scale factor is usually set to be 1.0, so it does not affect the fatigue results.
November 7, 2023 at 10:06 amFayçal ABDOUNFSubscriber
So I understood that FT is a post-processing step and then the FE stresses are not affected by it.
What I mean when I said that the results changed is that when I'm change the load and I keep the same history data in the FT, at the end, the results of the FT change, I will have more or less elements in red colors depending of the load I used in the static analysis.
I don't understand why we have a link between both because as we said, the load I put in the static is just serves to calculate the behavior of the part in terms of stresses to be used in the FT.
FY = 20N / Mapping FT
FY = 50 N
So what I understand is that the fatigue tool will take account of the static structural analysis we did before.
I thought that we can use a random value for the force in the static analysis.
November 7, 2023 at 2:08 pmDaniel ShawAnsys Employee
Yes, the fatigue calculations use the stress results from the static FE.
Stresses used in fatigue calculations = (FE stresses)*(multipliers in history data file)*(scale factor)
Increasing the load (and therefore increasing the calculated stresses) in the static FE, will increase the calculated fatigue damage.
November 7, 2023 at 2:25 pmFayçal ABDOUNFSubscriber
Then, as I have a history data, Do I have to take the first load of the history data (which is -80N for Fy or -80N for Fz here) to run the static and then I delete it from my table ?
Is it always the same process when you run a static analysis with the FT on workbench ? retrieving the first data of the history data file, use it as load in the static analysis and run FT.
November 7, 2023 at 2:32 pmDaniel ShawAnsys Employee
It is your decision about how to setup the analysis to create the correct stress history. A common approach is to apply a unit load in the FE (e.g., 1N) and then use the multipliers in the history data file to create the actual stress history, but that approach is not mandatory. You can also use real loads in the FE and the appropriate multipliers on those real loads in the history data file. You just have to keep in mind tha the stresses used in the fatigue calculations are the product of the FE stresses and the history data multipliers.
November 7, 2023 at 7:58 pmFayçal ABDOUNFSubscriber
Thank you so much for you explanation.
So, to check the model :
I switched the load to Fy=1N and I load the Fy history data file :
I get a life of 47 585 Cycles. But my damages are all over 1, they should be less than 1.
How can I use these damage results to determine after both analysis (with fy and fz) to determine the life in cycles using Miner's rule ?
In Apdl script I had a table with damage less than 1 and I add whole node damage to get the life.
November 10, 2023 at 6:30 amDaniel ShawAnsys Employee
What is the setting for "Design Life" in the Details Window. The default setting is probably 1e9 blocks. The damage reported by the FT is the traditional damage calculation multiplied by the specified Design Life. To obtain the damage value that you desire, you may want to set the Design Life to be 1 block,.
- 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.
- Saving & sharing of Working project files in .wbpz format
- Solver Pivot Warning in Beam Element Model
- 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
- 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
- Defining rigid body and contact
- Colors and Mesh Display
- A solver pivot warning or error has been detected
© 2023 Copyright ANSYS, Inc. All rights reserved.