

November 16, 2018 at 8:20 amsaimaaz786Subscriber
I have a bean which is given time series data of force ( Amplitude is not constant with time) for fatigue analysis. When i expand the fatigue tool for rain flow matrix ,it ask for History data. Now my is question, what is this History data ?? Is is it the applied time vs force data or some thing else??? Kindly help me.Thanking you

November 16, 2018 at 6:45 pmSandeep MedikondaAnsys Employee
Hi, From the manual:
The History Data option enables you to import a file containing the data points. This option is a nonconstant amplitude proportional loading type. This data is depicted in a graph on the Worksheet. You can specify the number of data points this graph will display using the Maximum Data Points To Plot property in the Options category.
Maximum Data Points To Plot
This option is only applicable for History Data loading and allows you to specify the number of data points to display in the corresponding graph that appears in the Worksheet. The default value is 5000 points. The graph displays the full range of points and all points are used in the analysis. However, depending on the value you set, every second or third point may not be displayed in the interest of avoiding clutter and making the graph more readable.
the time history file is ASCII file with a single column of data. The data are the load multipliers. For example, if you mount an accelerometer on a car axis, you can measure the g loading (say ever second) over some period of operation (1 day or typical use, 1 loop around a test track, etc.). Those g values can be stored in a load history file. You could then construct a FE model with a 1G loading. Multiplying the time history file by the 1G results produce a stress history that can be used to predict fatigue damage.
It is requested under the rainflow matrix option, because time history is the only loading mechanism in the Mechanical Fatigue Tool that produces a rainflow matrix.
Regards,
Sandeep 
November 17, 2018 at 1:45 am

November 17, 2018 at 6:23 amsaimaaz786Subscriber
Dear Sir ,
First of all I would like to thank you for giving me your precious time.I got some idea about that but still confused. Once again i would like to explain my problem .I have a cantilever beam which is subjected to Aerodynamic load at the free end . This force was applied in the form of table (Time vs Force ,Rows =6000 ,Column =2) under the transient in order to evaluate the fatigue damage. Problem arises when I try to get damage matrix/rain flow matrix as for that History data is needed. Sorry i am asking very stupid question , From where i will get this History data??? Is it the time history of force??? or tabular load(TIME Vs Force ) which was applied to the free end of cantilever ???

November 17, 2018 at 6:25 amsaimaaz786Subscriber
Dear Sir ,
First of all I would like to thank you for giving me your precious time.I got some idea about that but still confused. Once again i would like to explain my problem .I have a cantilever beam which is subjected to Aerodynamic load at the free end . This force was applied in the form of table (Time vs Force ,Rows =6000 ,Column =2) under the transient in order to evaluate the fatigue damage. Problem arises when I try to get damage matrix/rain flow matrix as for that History data is needed. Sorry i am asking very stupid question , From where i will get this History data??? Is it the time history of force??? or tabular load(TIME Vs Force ) which was applied to the free end of cantilever ???

November 17, 2018 at 4:12 pmpeteroznewmanSubscriber
Dear Saimaaz,
The History data is the time history of the 6000 rows of applied force. What are the units used in the table of force? Let's assume they are in kN.
Build a Static Structural model and apply a 1 kN force to this model. This represents a unit force. Solve it. ANSYS now knows the stress for a unit force. Import the 6000 rows of force data in kN. Each row in the table will be a scale factor on the stress result for the unit force of 1 kN. So if the table has a 2.2 in it then the stress will be for 2.2 kN and if the table has a 0.42 kN value, the stress will be multiplied by 0.42 to represent that row of the table. The Fatigue Tool will assemble the damage matrix/rainflow matix by binning the 6000 rows of scaled stress into a smaller number of bins.
I hope this makes sense.
Regards,
Peter 
November 18, 2018 at 7:11 amsaimaaz786Subscriber
Dear sir,
I followed your instruction as follow : (Please correct me if I am wrong )
Step 1 : I built static Structural model and applied a 1 kN force to the free end of the beam and ran the simulation.
Step 2: I Imported table (Time Vs Force history ) and applied to the free end of the beam and ran the simulation
Step 3: After step 2 , I opened fatigue tool for evaluating damage matrix /rainflow matrix .Here, under History data I attached Time history (Only) in the form of a text file and than reevaluated results.
Thanking you.

November 18, 2018 at 4:03 pmpeteroznewmanSubscriber
Dear Saimaaz,
Delete Step 2.
The results from Step 1 which has the 1 kN end load are used in Step 3 by the Fatigue Tool, along with a table of values of force in kN imported into the Fatigue Tool to compute the damage matrix / rainflow matrix.
Regards,
Peter 
November 19, 2018 at 6:56 pmsaimaaz786Subscriber
Dear Sir ,
Thank you Very much sir for your generous support. However, another sets of problems have emerged now. Sir, suppose I have a two different tables each having time force history and these tables are applied on the beam at the two different points. Now for computing damage matrix , which table shall i select for History data?? Because Under History data ,Its allowed to upload only one table.
Apart from this another questions is ,Is it possible to compute damage matrix/rain flow matrix in Mechanical APDL (Ansys 15.0) ??.
Thanking you
Regards
Saimaaz

November 19, 2018 at 7:50 pmpeteroznewmanSubscriber
Dear Saimaaz,
The Fatigue Tool is intended to simplify common calculations. You are describing an uncommon calculation that the Fatigue Tool was not designed to accommodate.
You should perform a Transient Dynamics simulation instead. Now both forces can be acting at the two locations over the duration of the test. You can output stress from as many locations as you want and perform a Fatigue Damage computation on each location.
Do you have matlab? There is a very useful and free GUI package called vibrationdata that includes Fatigue Damage calculations on timehistory data.
Regards,
Peter

 You must be logged in to reply to this topic.
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.
Ansys Blog
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
 An Unknown error occurred during solution. Check the Solver Output…..
 Understanding Force Convergence Solution Output
 Solver Pivot Warning in Beam Element Model
 Colors and Mesh Display
 How to calculate the residual stress on a coating by Vickers indentation?
 whether have the difference between using contact and target bodies
 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.
 User manual

2524

2066

1279

1096

457
© 2023 Copyright ANSYS, Inc. All rights reserved.