Impicit Delayed Norton Creep Implemented

Transcription

1 Impicit Delayed Norton Creep Implemented Carlos Shultz PADT Inc. Abstract A custom implicit creep routine was developed. The routine was based upon Norton's creep equation using Hoop Stress with an additional delay to the onset of creep. The delay, called an incubation time, was an exponential function of temperature and stress. The original implementation used Sz for 2D elements (182) and Sy for 3D element (85,186,187) but was extended to use Seqv. The procedure for compiling will be explained as well as other features including a verbose flag, a hoop vs. equivalent stress switch, and the use of state variables to track element status. Introduction A custom creep model, called a delayed Norton creep model, was implemented for use with ANSYS 8.1. Once the delay (a.k.a. incubation time) has been passed, each element is allowed to creep according to a Norton creep equation. The model is designed to use hoop stress (Sz when axi-symmetric and Sy when solid) or Seqv to calculate the amount of creep which occurs. Material Model Creep Strain Material specific constants C1 through C3 were used in the calculation of creep strain using the following equation: ε = C 1 S C hoop, avg 2 e C 3 T ε is the incremental creep strain T is absolute temperature, K S, is hoop stress in MPa hoop avg t t is the incremental time for the iteration Values of C1, C2, and C3 were: C1=0.15 C2=1.2 C3= Creep strain does not accumulate until incubation time has been exceeded.

2 Incubation Time Material specific constants C5 through C9 were used in the calculation of incubation time using the following equation: t inc = C 5 e C6 + C 8.314T 7 S hoop avg, ( C8 C9T ) 6 10 tinc is the incubation time T is absolute temperature, K S, is hoop stress in Pa hoop avg Values of C5 through C9 were: C5=0.003 C6= C7=2 C8=0.6 C9= Hoop vs. Equivalent Stress Toggle If C10 is set to 1 then the incubation time and creep strain calculations are based upon equivalent stress rather than hoop stress. This is implemented in the code like this: if (prop(10).eq.1) then tinc=c5 * exp(c6/8.314/t) * exp(c7*(c8-c9*t)*seqv/1e6) else tinc=c5 * exp(c6/8.314/t) * exp(c7*(c8-c9*t)*abs(shoopavg)/1e6) endif Usercreep.F Code Features Element Error Trapping and Hoop Stress Calculation The code was implemented for a subset of the elements in ANSYS. The code determines whether the element is allowed and if so, calculates the proper hoop stress. ival=elmget(elemid,elmdat,nodes) ival=etyget(elmdat(2),ielc(1)) Retrieve element type number Retrieve element type for the element type number

3 ival=ensget(elemid,stress) Retrieve nodal stress results If the element type is not supported, the code writes: UNSUPPORTED ELEMENT TYPE to the output window and goes to the end of the subroutine. If the axisymmetric keyoption is not specified, the code writes: FOR CUSTOMCREEP WITH TYPE 182 KEYOPT(3) MUST = 1 to the output window and goes to the end of the subroutine. The Hoop stress is calculated differently for each element type, for type 182, Sz for the corner nodes are stored in the 3 rd, 14 th, 25 th, and 36 th position of the stress array. So, the hoop stress is: S hoop, avg stress = () 3 + stress( 14) + stress( 25) + stress( 36) State Variables 4 State variables were used to track the state of the elements. If the incubation time for a given element has been exceeded, its 1 st state variable changes from 0 to 1. The state variables for all integration points of an element change in unison to prevent element distortion failures which occur if the element creeps at a subset of integration points. This is implemented in code like this: if (statedata(elemid,kdinpt).ne.1.0) then if (time.ge.tinc) then if incubation time exceeded, set flags and allow creep statev(1)=1.0 do 101 b=1,20 statedata(elemid,b)= continue else goto 990 otherwise skip creep endif endif Each elements 2 nd state variable contained the initial value of incubation time. Both of the variables can be printed and displayed during post-processing if outres,svar,all is entered prior to solution. Figures 1 through 3 below show a chronology of plots of SEQV and State Variable 1 side-by-side for 3 times during a sample analysis. The hollow cylinder in the example is loaded with internal pressure and axial tensile forces. Creep starts in the necked down region and spreads to other parts of the model as incubation time is passed.

4 Figure 1. Plot of SEQV and State at time=3262, incubation time > 3262 in all elements Figure 2. Plot of SEQV and State at time=3518, incubation time exceed in some elements

5 Figure 3. Plot of SEQV and State at time=34048, incubation time exceed in more elements Verbose Flag To print out information regarding the current calculations to the output window a verbose flag was implemented. The user sets material property 4 to 1 in order to trigger output printing. The code to implement this is: if (prop(4).eq.1) then write (6,991) elemid,elmdat(2),ielc(2),ielc(5),elmdat(5) 991 format ('elemid: ',I8,' typenum: ',I3,' type&key3: ',I3,1x,I1,' esys: ',I2) write (6,992) t,temp,toffst 992 format ('abs_temp: ',F12.3,' temp: ',F12.3,' temp_off: ',F12.3) etc endif The verbose flag simplifies both debugging during development and post-compile verification as the user does not need to recompile in order to use this feature.

6 Compiling Procedure for compiling Make sure that you load the customization tools when installing ANSYS. Figure 4 below shows an example of the installation gui. Figure 4. Installation gui example showing customization tools option You must have the correct Fortran Compiler available. For ANSYS 8.1 windows 32bit, the version is Compaq Visual Fortran Standard Edition 6.6A. Run the provided anscust.bat file which is in this directory for a standard installation: C:\Program Files\Ansys Inc\v81\ANSYS\custom\user\intel Figures 5,6 and 7 show the expected output when running the anscust.bat file.

7 Figure 5. Anscust.bat will compile all of the fortran code in the directory and then link the resulting objects with the precompiled objects Figure 6. A successful linking will look like this

8 Figure 7. In the compiling directory you will have a custom ANSYS executable as shown in this image Using the custom ANSYS executable To launch ANSYS using the custom executable, use the customization tab of the launcher. Use the browse button to navigate to the proper file and then point at the ANSYS.exe file as shown in figure 8 below. Figure 8. Launcher showing the customization tab and use of the Custom ANSYS.exe If all has gone properly you should see the following in the output window, see figure 9, Note This ANSYS version was linked by Licensee. Figure 9. Output window indicates that the user has linked the version of ANSYS being used Using the custom material model To use the custom creep model, use the material selection gui, select Creep and State Variables as shown in figures 10 and 11. Add rows for the 10 constants and add temperatures as desired. Enter the data and then press OK. Enter zeros for the state variables.

9 Figure 10. Material Definition GUI showing where to specify custom creep model parameters. Figure 11. Material Definition GUI showing where to specify custom creep model parameters. Alternatively, you can enter the data using APDL like this:

10 TB,CREEP,1,2,10,100 TBTEMP,1300 TBDATA,1,0.15,1.2, ,0 TBDATA,5,0.003,180000,2,.6, TBDATA,10,0 TBTEMP,1500 TBDATA,1,0.15,1.2, ,0 TBDATA,5,0.003,180000,2,.6, TBDATA,10,0 TB,STATE,1,,2 Model Verification A variety of test cases were run. One case set incubation time to 0 to compare against the built in implementation of Norton s creep. Another case was run with constant stress and compared to hand calculations.