Set Up the Fatigue Analysis

Fatigue Quick Start Guide > Component S-N Analysis > Set Up the Fatigue Analysis

XXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXX''">XXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXX''">

To begin setup for a fatigue analysis, press the Analysis switch in Pre & Post (or from the Tools pull-down menu in MSC Patran, select MSC Fatigue and then Main Interface). This will bring up the MSC Fatigue main form from which all parameters, loading and materials information, and analysis control are accessed.

Once the form is open, set the General Setup Parameters as follows:

1. Analysis: S-N

2. Results Loc.: Node

This simply means that the fatigue lives will be determined at the nodes of the model.

3. Nodal Ave.: Global

Accept the default which simply means element nodal stresses will be averaged to the nodes.

4. F.E. Results: Stress

S-N analyses require stresses; you do not have a choice.

5. Res. Units: PSI

Model dimensions are inches and forces are in Pounds, therefore stress units are PSI.

6. Jobname: comp_sn

7. Title: Component S-N Analysis

Solution Parameters

Open the Solution Params... form. On this form leave all the defaults except:

Certainty of Survival: 96

As we learned in the last exercise, the S-N data can have significant scatter associated with it. We are asking MSC Fatigue to calculate a fatigue live with 96% certainty of survival based on the scatter in the S-N data. This corresponds to a 4% failure rate.

Click the OK button to continue.

Material Information

The component was tested under constant amplitude, fully-reversed conditions to produce S-N data. In the previous examples we have used S-N curves that are representative of the material and independent of geometry. They related local stress (σ) to life. Now we have a different situation where the actual component geometry itself as well as the material has been used in tests to create the S-N curve. This type of S-N curve is called a component S-N curve. These type of curves relate nominal stress (S) to life and are dependent on the geometry of the component. If you change the geometry, the curve will no longer be valid. The nominal stress is a location away from the actual failure location. This is usually because it is impossible to place a measurement device such as a strain gauge in the failure location. The stress for the S-N curve was measured using strain gauges at a point one quarter of an inch from the weld on the main bar and 5 inches from each end of the bar. Node 514 of the model corresponds to this measurement point for the S-N curve. The point of measurement is sometimes referred to as the reference location.

For this model we have an S-N curve that needs to be input to PFMAT, the materials database manager. Two methods of entering this data will be given.

Table 4‑2 S-N Data Set for Bracket Assembly
Properties	SI	Imperial
S-N Properties:
Stress Range Intercept, SRI1	10,710 MPa	1553 KSI
First fatigue strength exponent, b1	-0.33333	-0.33333
Fatigue transition point (cycles), NC1	1E7	1E7
Second fatigue strength exponent, b2	-0.2	-0.2
Standard error of Log (N), SE	0.2	0.2
R-Ratio of test, RRAT	-1	-1
Monotonic Properties:
Young’s Modulus, E	205,800 MPa	29, 850 KSI
UTS	700 MPa	101.5 KSI

Manual Entry of Materials Data

Open the Material Info... form and press the Materials Database Manager button. This will invoke PFMAT. Once the program has started, select Create | data set 1.

You will be asked for a password to modify the central database location. If you do not enter a password and simply press the carriage return or the OK button, a copy of the central materials database will be copied to your local directory where you can then proceed to enter your materials data.


Note:	PFMAT always tells you at the top of its main menu whether it is connected to the central database in the MSC Fatigue installation area or a local database in the current directory, or even some other database that you may have created in another directory.

Now a series of forms will open requesting data entry. On the first form, Names, enter:

1. Primary name: BRACKET_SN

2. Anything else you want - not required

On the next form, Static Data, enter the generic (monotonic) information:

1. UTS: Ultimate Tensile Strength (MPa): 700

2. E: Elastic modulus (MPa): 205800

Only these two parameters are required to be entered. The next form (E-N data) is for strain data. Skip over this form by clicking the OK button. The next form is for S-N data. Select Component from the pull-down menu.

For the rest of the data, enter the SI values as indicated in Table 4‑2. Click the OK button when done. Fracture Mechanics Data is requested next. Just click the OK button to skip over this. Multiaxial data is requested next. Skip over this form also by clicking the OK button. The material will be entered into the database. Press or double-click the Graphical Display switch to view the S-N curve.


Hint:	We are entering the data here in SI units. All underlying fatigue calculations are done using SI units. However if you wish to enter and view materials data in Imperial units, set the preference using Preferences \| Stress units \| PSI. You can save this setting globally, or just locally in your working directory (or not at all) so that each time you invoke PFMAT it remembers to display values and plots in your units of preference.


Note:	S-N curves are characterized by a power law and thus appear as straight lines in log-log space. The equation is S=SRI1(N)b where SRI1 is the y-intercept and b is the slope (after Basquin). It is interesting to note historically that, although invented in 1870 by August Woehler, the S-N curve was not actually displayed graphically until some 30 years later. And it was not until 10 years after that that the curves were characterized in equation form. Our curve actually has two slopes and a transition point. If the second slope were zero it would act as a fatigue limit.

Exit from PFMAT when you are done using the File | Exit and the eXit switch.

Batch Entry of Materials Data

Input another S-N data set. To illustrate batch mode operation of PFMAT we are going to define the parameters of the second S-N set in a file. Using your a text editor, create a file called bracket.mat in the working directory.

Table 4‑3
S-N Properties	SI	Imperial
Stress Range Intercept, SRI1 (MPa)	13950	2023ksi
Slope, b1	-0.29	-0.29
Transition life, NC1 (cycles)	2E7	2E7
Slope, b2	-0.16	-0.16
Standard error, SE	0.14	0.14
Stress ratio, RRAT	-1	-1

Enter the following lines in this file:

/OPT=CREATE
/INDB=YES
/PASS=
/MATNO=2
/PRI=BRACKET_SN2
/UTS=700
/E1=205800
/SNT=C
/SRI=13950
/B1=-0.29
/NC1=2E7
/B2=-0.16
/SE=0.14
/RRAT=-1
/OPT=EX

Then from the system prompt or a DOS window issue the following command:

pfmat @bracket.mat

ASCII Materials File Reader

The MAT file created above can also be entered in the S-N data set by using the ASCII Materials File Reader. This form can be accessed by going to the Tools pull-down menu and selecting MSC Fatigue (for the MSC Patran version) or Fatigue Utilities (for the Standalone version). From here, select Material Management and then ASCII Materials File Reader.

On the form that comes up, enter the name bracket.mat into the MAT Filename databox and click the Apply button.


Note:	The above mentioned MAT file can also be created from scratch by using the “Edit” button on the form shown above.

Either of the above mentioned two methods will put the second data set into the database. Graphically compare bracket_sn and bracket_sn2 by running PFMAT interactively and using the Graphical display option. To run interactively you can either just type pfmat at the system prompt or go back to Pre & Post or MSC Patran and spawn it from the MSC Fatigue Material Info... form. Make sure both bracket_sn and bracket_sn2 are loaded as data set 1 and 2 using Load | data set n.


Hint:	If you do not have any S-N data, but only know E and UTS, you can have PFMAT generate generic material properties based on empirical formulas and the type of material. Simply enter E and UTS as if you were going to enter your own S-N data and the Material Type Number (see the MSC Fatigue User’s Guide) and the S-N parameters will be generated automatically for you. (99=steel of unknown heat treatment) Of course you have to turn on the Generate all parameters from UTS toggle.

Specify the Material for the Analysis

On the Material Info... form enter the following in the spreadsheet:

1. Material: BRACKET_SN

Select the cell under the Material column to activate it and select the S-N curve from the listbox that appears below the spreadsheet. The next cell will become active.

2. Finish: No Finish

Select No Finish from the pull-down menu that appears below the spreadsheet. Finish and treatment are not allowed in a component S-N analysis (they are built into the curve). They will be ignored if you set them. The next cell will become active once you select the finish.

3. Treatment: No Treatment

Select No Treatment. The next cell becomes active.

4. Region: default_group

Select default_group which contains the nodes and elements from the entire model.

Close the Material Info... form when you are done by clicking OK.

Loading Information

To create the time history which represents the actual loading conditions of the bracket, use PTIME and the X-Y points option representing y-values only. The time history will have a maximum of 3000 lbs and a minimum of –7000 lbs. No other information has been given so you can assume that there are no peaks and valleys between these points and that only these two points are required. You will enter the values 0, 3000, –7000, and 0 to create this loading.

The 1/2 hour interval can be modeled using the fatigue equivalent units. This is a term relating to the real value of one repeat of the time history. In this case, you can use 30 minutes, 1/2 hours, 1/48 days, etc. The answer will be the same of course, but you can choose the best parameter for reporting the life of your product.

Open the Loading Info... form and click the Time History Manager button.

Define the Load

When PTIME comes up, select Enter X-Y points as the method of input.


Note:	If you have been working sequentially through this document, then you will already have some entries in the PTIME database. The version of the form that is displayed will be different than the one shown here. On this form, select Add an entry and then select the option X-y time series, which is the equivalent of selecting Enter X-Y points on the shown form.

A form will appear that will ask for a name, description and other information. Enter the following leaving defaults for those not mentioned:

1. Filename: BRACKET_LOAD

2. Description 1: Bracket Loading

3. Load Type: Force

4. Units: lbs force

5. Number of fatigue equivalent units: 0.5

6. Fatigue Equivalent Units: Hours

We are defining a single occurrence of this signal as representing 1/2 hour.

Click the OK button to go on. Next you will be prompted to enter the Y points. Enter the following numbers with a carriage return after each: 0, 3000, -7000, 0. End by putting in a blank entry and then click the End button.

Plot the Time History

PTIME returns to its main menu where you can select Plot an entry to make sure it took correctly. Accept the default file, BRACKET_LOAD.

Select File | Exit to close the plot and press or double-click the eXit switch in PTIME.

Associate the FE Load to its Time Variation

Now back on the Loading Info... form you must associate the time variation of the load that you just created to the FE load case. Go to the spreadsheet as was done in the previous example. Select the first cell with the mouse to activate it.

1. Load Case ID: 1.1-3.1-1-

This is the internal database ID. You select the FE results from the listboxes below. You must select a Result Case, a Stress result, and a layer. Then you click the Fill Cell button to enter it in the spreadsheet cell. The listboxes may appear empty at first. To fill them select the Get/Filter Results... button and turn ON the Select All Result Cases toggle and click Apply.


Note:	The load case ID may be different than that shown here.

2. Time History: BRACKET_LOAD

The middle cell should become active after selecting the FE result. Another spreadsheet appears at the bottom of the form from which you select the time history file. Click on the BRACKET_LOAD row anywhere with the mouse. This will fill the cell with the time history file name.

3. Load Magnitude: 900

The next cell becomes active and a databox appears below the spreadsheet. Change this entry to 900. You must press a carriage return (Return or Enter) to accept the value in the databox below the spreadsheet. A common mistake is to forget to press the carriage return to accept the value. Remember we are normalizing the FE stresses by dividing by the total applied load magnitude of 900 lbs from the FE analysis to simulate a stress distribution due to a unit load. The time variation represents the actual load magnitudes.

The time variation of the loading is now associated to the static FE results. Click the OK button to close the Loading Info... form.