Permalink Submitted by chau on Sun, 2007-02-25 07:00.
Dear,
I want to make a code for central crack plate under the impulsive load by Ansys.
My difficult proplem is make the impulsive loading (Step load) (Trainsient dynamic Full mode) such as the tensile load P(t) = 4000 N/m2 for a plate has a central crack (see above figure), and I want to get the dynamic stress intensity factors with time. I can solve the same problem under static load and I can find the SIFs KI by Ansys. But for impulsive load, I have not yet known to input the load and get DSIFs with time.
So, if every member has the Ansys code such as a plate has a hole under the impulsive loading, please give me to I can read it to learning.
I am also trying to solve a similar problem using ANSYS but have been unsuccessful so far at applying an impulse load as well as a static load.
I have done a tutorial which applies a short pulse load to a 1D beam.
My current 2D fracture model is under a static load but ANSYS will not calculate the SIF because I keep getting an error about the x-axis not being parallel to the crack face.
If you have recieived any advice on your problem, can you be so kind as to share the knowledge ? :)
To avoid the "x-axis not being parallel to the crack face" error you may create a local coordinate (LOCAL command) system with the x direction over the symmetry plane pointing to the remaining ligament of the material, the y direction must be oriented in the same direction as the applied load. The origin must be placed at the crack tip.
You can find more detailed information in Ansys documentation- Structural analysis guide - fracture mechanics - calculating fracture mechanics. A useful tutorial can be found at
dl,3,1,symm dl,5,1,symm dtran ANTYPE,TRANS ! FULL TRANSIENT DYNAMIC ANALYSIS finish
finish /SOLU SOLCONTROL,0 KBC,1 ! STEP BOUNDARY CONDITIONS TIME,1e-2 sfl,2,pres,-100 sftran ! TIME AT THE END OF LOAD STEP 1 NSUBST,50 ! 10 SUBSTEPS FOR TIME STEP OF .0004 OUTPR,BASIC,1 ! PRINT BASIC SOLUTION FOR EACH SUBSTEP OUTRES,ESOL,1 ! STORE Element SOLUTION FOR EACH SUBSTEP OUTRES,NSOL,1 ! STORE NODAL SOLUTION FOR EACH SUBSTEP SOLVE FINISH
/POST26 NSOL,2,65,U,Y,UY ! STORE UY DISPLACEMENTS OF NODE 1 AGAINST TIME PRVAR,2 ! PRINT VARIABLE 2 (DISPLACEMENT UY OF NODE 1) V/S TIME /GRID,1 ! TURN THE GRID ON FOR DISPLAY /AXLAB,Y,DISPLACEMENT ! MAKE Y-AXIS LABEL AS DISP FOR DISPLAY PLVAR,2
/OUTPUT /POST1 ETABLE,SENE,SENE ! RETRIEVE STRAIN ENERGY PER ELEMENT ETABLE,VOLU,VOLU ! RETRIEVE VOLUME PER ELEMENT C*** IN POST1 DETERMINE KI (STRESS INTENSITY FACTOR) USING KCALC !** PATH,KI1,3,,48 ! DEFINE PATH WITH NAME = "KI1" PPATH,1,46 ! DEFINE PATH POINTS BY NODE PPATH,2,57 PPATH,3,54 KCALC,,,1 ! COMPUTE KI FOR A HALF-MODEL WITH SYMM. B.C. *GET,KI1,KCALC,,K,1 ! GET KI AS PARAMETER KI1
!dl,3,1,symm !dl,5,1,symm !dtran nsel,, loc, x, 0.0, W nsel, r, loc, y, 0.0, 0.0 dsym, symm, y nsel, , loc, x, -a, -a dsym, symm, x alls ANTYPE,TRANS ! FULL TRANSIENT DYNAMIC ANALYSIS finish
finish /SOLU SOLCONTROL,0 KBC,1 ! STEP BOUNDARY CONDITIONS ALPHAD,0.00007 ! EQUIVALENT STRUCTURAL DAMPING ALPHA BETAD,.000000015 ! EQUIVALENT STRUCTURAL DAMPING TIME,15e-6 ! END TIME sfl,2,pres,-400 ! PRESS ON THE TOP EDGE OF THE PLATE sftran ! TIME AT THE END OF LOAD STEP 1 NSUBST,200 ! 200 SUBSTEPS FOR TIME STEP OF .0004 OUTPR,BASIC,1 ! PRINT BASIC SOLUTION FOR EACH SUBSTEP OUTRES,ESOL,1 ! STORE Element SOLUTION FOR EACH SUBSTEP OUTRES,NSOL,1 ! STORE NODAL SOLUTION FOR EACH SUBSTEP SOLVE FINISH
You might be interested these papers, particularly, the first one.
1. Xie D and Biggers, Jr. SB, Calculation of transient strain energy release rate under impact loading based on virtual crack closure technique, International Journal of Impact Engineering, 34(2007): 1047-1060.
2. Qian Q and Xie D, Analysis of mixed-mode dynamic crack propagation by interface element based on virtual crack closure technique, Engineering Fracture Mechanics, 74(2007): 807-814.
To my experience, most commercial FEA codes didn't implement fracture mechanics in a good manner. So , if you really want to do something on fracture analysis, you'd better develop something yourself. Otherwise, you will continue suffering from using those fracture analysis features provided by commercial FEA codes.
However, if you simply want to get a short assignment done quickly, that's another story.
Dear Prof, Thank you very much for your respond.I have read two that papers on web www.sciencedirect.com and it is very important to me because from that i can get the dynamic stress intensity factors (KI and KII). I have the code on C++ which the crack propagates at constant in homogeneous material under mode I loading. This code uses Virtual Crack Closure Technique (VCCT) to get the dynamic stress intensity factors but because for mode I, the energy releases rates is limited by the Rayleigh wave speed (Freund 1990). This code can apply for mixed mode loading of crack propagates at constant speed.So, i want to know why under mode I, why is the crack velocity limited by the Rayleigh wave speed? and if in kinking case, why are we not apply this method (VCCT)? And final, I have not yet understood in your sample in the paper "Analysis of mixed-mode dynamic crack propagation by interface element based on virtual crack closure technique" because if with that initial crack direction, loading and constraints, I think the direction of crack propagation will straight (perpendicular to the right line of the plate). Would you please explain to me some my above wonderings.Thank you very much.
I am not proficient in ANSYS but i have tried calculating the DSIFs using BEM, the DSIFs can be calculated using the crack opening displacements. If you can use ANSYS to determine the crack opening displacements, then you can use the equations to calculate those.
regards,
alan
P.S. I am new in here and hopefully i can learn as well as help here.
Thank you for interested. Actually, you raised very good questions. Since I'm on leaving to Honolulu for a AIAA confernce, I have no time to response right now. Also let me think a while. Please be back a week later.
Aloha! I'm back and I try to answer your questions:
1. So, i want to know why under mode I, why is the crack velocity limited by the Rayleigh wave speed?
This is predicted from the math model. For a crack in an inifite body subjected to mode I loading at remote, the crack velocity can be derived based on the energy balance. Two milestones are:
If you set crack length "a" to infinity, you can find the crack velocity limits as
Mott: V ->0.38*C0
Freund: V->Cr
Therefore, from Freund's model, the crack velocity is limited by Rayleigh Wave speed. This is what you said.
However, from Mott's model, the crack velocity V is limited by 0.38C0. More test data support Mott's model though, it is the oldest one.
Some other models were also proposed. Recently, Prof. W Yang (Tsinghua University, China) and Prof. H Gao (Plant Max, Germany) did predictions that the crack velocity can exceed Cr. Prof. Rosakis (Caltech, USA) confirmed this throuth tests. If you have further interests, you may consult them.
In brief, the statement of "crack velocity is limited by Rayleigh wave speed" is a math model prediction based on energy balance.
2. and if in kinking case, why are we not apply this method (VCCT)?
The popular VCCT works for selfsimilar cracks. In other words, crack must extend along its original orietation. For kinking, the crack suddenly changes its direction, and a modified version of VCCT is needed. Some detailed discussions can be found in my papers, particularly the first one:
1. Xie D, Waas AM, Shahwan KW, Schroeder JA and Boeman RG, Computation of strain energy release rate for kinking cracks based on virtual crack closure technique, CMES: Computer Modeling in Engineering & Sciences, 6(2004): 515-524.
2. Xie D, Waas AM, Shahwan KW Schroeder JA, and Boeman RG, Fracture criteria for kinking cracks in triple material bonded joints, Engineering Fracture Mechanics, 72(2005): 2487-2504. (Science Direct Top 25 Hottest Articles, #3, Jul-Sep, 2005, #13, Oct-Dec, 2005)
3. And final, I have not yet understood in your sample in the paper "Analysis of mixed-mode dynamic crack propagation by interface element based on virtual crack closure technique" because if with that initial crack direction, loading and constraints, I think the direction of crack propagation will straight (perpendicular to the right line of the plate). Would you please explain to me some my above wonderings.Thank you very much.
Your thinking is absolutely right. Actually, the test observations support your saying. This is because that cracks always like to propagate in pure mode I locally.
In this example, the crack was forced to grow along a predefined crack path so that make it mixed-mode. In reality when you test it, it may not propagate that way. I chose this example because it was simulated by Profs. Atluri and Nishioka by using their moving singular elements and thus I was able to verify my UEL implementation. And also want to see if this kind of problems can be simulated in a much simpler way.
In brief, this is just simply a math example to verify codeing.
Hopefully my answers could be some kind of help to you.
I have similar problem with Chau. I am able to get the stress intensity factor for static loading, but for transient, I was unable to get my stress intensity factor with respect to time using POST26.
I wanted to get some insight in the transient stress intensity factor (SIF).
In the time history, we notice there is an overshoot (~27%) from the
steady state SIF for a fixed (not propagating crack). I found the
overshoot occurs at the time when the reflected wave from the opposite
crack-tip comes back to the first crack tip. I wanted to know why this
overshoot occurs, what is the physical explanation?
I also have this problem of getting ANSYS to list the results of the stress intensity factors against time,i was wondering whether could anyway give me some tips on how to progress. I am really stuck in a rut. Please help. Your help will be very much appreciated. Thank you.
pls tell me the stepwise procedure to create crack in the beam and also crack open and close in the cantilever beam in ansys mechanical apdl..how u write alogorithm in ansys window to run a program as soon as possible..in my email-swagatmahata.337@gmail.com
Comments
Make a code for central crack plate under the impulsive load
Dear,
I want to make a code for central crack plate under the impulsive load by Ansys.
My difficult proplem is make the impulsive loading (Step load) (Trainsient dynamic Full mode) such as the tensile load P(t) = 4000 N/m2 for a plate has a central crack (see above figure), and I want to get the dynamic stress intensity factors with time. I can solve the same problem under static load and I can find the SIFs KI by Ansys. But for impulsive load, I have not yet known to input the load and get DSIFs with time.
So, if every member has the Ansys code such as a plate has a hole under the impulsive loading, please give me to I can read it to learning.
Thank you very much,
Best Regards,
Chau
Dear Chau, I am also trying
Dear Chau,
I am also trying to solve a similar problem using ANSYS but have been unsuccessful so far at applying an impulse load as well as a static load.
I have done a tutorial which applies a short pulse load to a 1D beam.
My current 2D fracture model is under a static load but ANSYS will not calculate the SIF because I keep getting an error about the x-axis not being parallel to the crack face.
If you have recieived any advice on your problem, can you be so kind as to share the knowledge ? :)
Thank you.
Regards,
Idris
ANSYS SIF
Dear Idris,
To avoid the "x-axis not being parallel to the crack face" error you may create a local coordinate (LOCAL command) system with the x direction over the symmetry plane pointing to the remaining ligament of the material, the y direction must be oriented in the same direction as the applied load. The origin must be placed at the crack tip.
You can find more detailed information in Ansys documentation- Structural analysis guide - fracture mechanics - calculating fracture mechanics. A useful tutorial can be found at
http://www.southalabama.edu/engineering/mechanical/faculty/phan/ANSYS_LE...
Unfortunately I have no experience with impulse loads in ANSYS. I hope you find this information useful.
All the best,
Allan Burke
Same Problem
Dear Chau,
I am facing the same problem as you do. Hope you can advise on how to display mi KI on post26
Thank you
Regards,
Huang
Ansys
finsh
/clear
L=10
a=6
W=26
radius=0.1*a
nu=0.286
young=76E9
pi=acos(-1)
/Prep7
mp,ex,1,young
mp,nuxy,1,nu
mp,dens,1,2450
et,1,plane82
keyopt,1,3,3
r,1,1
ptxy, 0, 0, -a, 0, -a, L, W-a, L
ptxy, W-a, 0
poly
lesize, 1, , , 10, 8
lesize, 3, , , 10, 1/8
lesize, 4, , , 4
lesize, 5, , , 8
kscon, 5, radius
amesh,1
dl,3,1,symm
dl,5,1,symm
dtran
ANTYPE,TRANS ! FULL TRANSIENT DYNAMIC ANALYSIS
finish
finish
/SOLU
SOLCONTROL,0
KBC,1 ! STEP BOUNDARY CONDITIONS
TIME,1e-2
sfl,2,pres,-100
sftran ! TIME AT THE END OF LOAD STEP 1
NSUBST,50 ! 10 SUBSTEPS FOR TIME STEP OF .0004
OUTPR,BASIC,1 ! PRINT BASIC SOLUTION FOR EACH SUBSTEP
OUTRES,ESOL,1 ! STORE Element SOLUTION FOR EACH SUBSTEP
OUTRES,NSOL,1 ! STORE NODAL SOLUTION FOR EACH SUBSTEP
SOLVE
FINISH
/POST26
NSOL,2,65,U,Y,UY ! STORE UY DISPLACEMENTS OF NODE 1 AGAINST TIME
PRVAR,2 ! PRINT VARIABLE 2 (DISPLACEMENT UY OF NODE 1) V/S TIME
/GRID,1 ! TURN THE GRID ON FOR DISPLAY
/AXLAB,Y,DISPLACEMENT ! MAKE Y-AXIS LABEL AS DISP FOR DISPLAY
PLVAR,2
Ansys static
L=20
a=4
W=10
radius=0.1*a
nu=0.3
young=210e9
pi=acos(-1)
/Prep7
mp,ex,1,210e9
mp,nuxy,1,0.3
mp,dens,1,7800
et,1,plane82
keyopt,1,3,3
r,1,1
ptxy, 0, 0, -a, 0, -a, L, W-a, L
ptxy, W-a, 0
poly
lesize, 1, , , 10, 8
lesize, 3, , , 10, 1/8
lesize, 4, , , 4
lesize, 5, , , 8
kscon, 5, radius
amesh,1
dl,3,1,symm
dl,5,1,symm
dtran
sfl,2,pres,-1000
sftran
ANTYPE,0
finish
/solu
solve
finish
/OUTPUT
/POST1
ETABLE,SENE,SENE ! RETRIEVE STRAIN ENERGY PER ELEMENT
ETABLE,VOLU,VOLU ! RETRIEVE VOLUME PER ELEMENT
C*** IN POST1 DETERMINE KI (STRESS INTENSITY FACTOR) USING KCALC !**
PATH,KI1,3,,48 ! DEFINE PATH WITH NAME = "KI1"
PPATH,1,46 ! DEFINE PATH POINTS BY NODE
PPATH,2,57
PPATH,3,54
KCALC,,,1 ! COMPUTE KI FOR A HALF-MODEL WITH SYMM. B.C.
*GET,KI1,KCALC,,K,1 ! GET KI AS PARAMETER KI1
Impule loading with damping ( C = alpha*M+beta*K)
L=20e-3
a=6e-3
W=10e-3
radius=0.1*a
nu=0.3
young=210e9
pi=acos(-1)
/Prep7
mp,ex,1,210e9
mp,nuxy,1,0.3
mp,dens,1,7800
et,1,plane82
keyopt,1,3,3
r,1,1
ptxy, 0, 0, -a, 0, -a, L, W-a, L
ptxy, W-a, 0
poly
lesize, 1, , , 10, 8
lesize, 3, , , 10, 1/8
lesize, 4, , , 4
lesize, 5, , , 8
kscon, 5, radius
amesh,1
!dl,3,1,symm
!dl,5,1,symm
!dtran
nsel,, loc, x, 0.0, W
nsel, r, loc, y, 0.0, 0.0
dsym, symm, y
nsel, , loc, x, -a, -a
dsym, symm, x
alls
ANTYPE,TRANS ! FULL TRANSIENT DYNAMIC ANALYSIS
finish
finish
/SOLU
SOLCONTROL,0
KBC,1 ! STEP BOUNDARY CONDITIONS
ALPHAD,0.00007 ! EQUIVALENT STRUCTURAL DAMPING ALPHA
BETAD,.000000015 ! EQUIVALENT STRUCTURAL DAMPING
TIME,15e-6 ! END TIME
sfl,2,pres,-400 ! PRESS ON THE TOP EDGE OF THE PLATE
sftran ! TIME AT THE END OF LOAD STEP 1
NSUBST,200 ! 200 SUBSTEPS FOR TIME STEP OF .0004
OUTPR,BASIC,1 ! PRINT BASIC SOLUTION FOR EACH SUBSTEP
OUTRES,ESOL,1 ! STORE Element SOLUTION FOR EACH SUBSTEP
OUTRES,NSOL,1 ! STORE NODAL SOLUTION FOR EACH SUBSTEP
SOLVE
FINISH
Papers on this topic
You might be interested these papers, particularly, the first one.
1. Xie D and Biggers, Jr. SB, Calculation of transient strain energy release rate under impact loading based on virtual crack closure technique, International Journal of Impact Engineering, 34(2007): 1047-1060.
2. Qian Q and Xie D, Analysis of mixed-mode dynamic crack propagation by interface element based on virtual crack closure technique, Engineering Fracture Mechanics, 74(2007): 807-814.
To my experience, most commercial FEA codes didn't implement fracture mechanics in a good manner. So , if you really want to do something on fracture analysis, you'd better develop something yourself. Otherwise, you will continue suffering from using those fracture analysis features provided by commercial FEA codes.
However, if you simply want to get a short assignment done quickly, that's another story.
Good luck!
Virtual crack closure technique to get DSIFs
Dear Prof, Thank you very much for your respond.I have read two that papers on web www.sciencedirect.com and it is very important to me because from that i can get the dynamic stress intensity factors (KI and KII). I have the code on C++ which the crack propagates at constant in homogeneous material under mode I loading. This code uses Virtual Crack Closure Technique (VCCT) to get the dynamic stress intensity factors but because for mode I, the energy releases rates is limited by the Rayleigh wave speed (Freund 1990). This code can apply for mixed mode loading of crack propagates at constant speed.So, i want to know why under mode I, why is the crack velocity limited by the Rayleigh wave speed? and if in kinking case, why are we not apply this method (VCCT)? And final, I have not yet understood in your sample in the paper "Analysis of mixed-mode dynamic crack propagation by interface element based on virtual crack closure technique" because if with that initial crack direction, loading and constraints, I think the direction of crack propagation will straight (perpendicular to the right line of the plate). Would you please explain to me some my above wonderings.Thank you very much.
DSIF's
I am not proficient in ANSYS but i have tried calculating the DSIFs using BEM, the DSIFs can be calculated using the crack opening displacements. If you can use ANSYS to determine the crack opening displacements, then you can use the equations to calculate those.
regards,
alan
P.S. I am new in here and hopefully i can learn as well as help here.
I'll answer you a week later
Chau,
Thank you for interested. Actually, you raised very good questions. Since I'm on leaving to Honolulu for a AIAA confernce, I have no time to response right now. Also let me think a while. Please be back a week later.
Thanks,
De
Aloha! I'm back and I try to
Aloha! I'm back and I try to answer your questions:
1. So, i want to know why under mode I, why is the crack velocity limited by the Rayleigh wave speed?
This is predicted from the math model. For a crack in an inifite body subjected to mode I loading at remote, the crack velocity can be derived based on the energy balance. Two milestones are:
Mott (1948): V=0.38*C0*(1-ac/a)
Freund (1972): V=Cr*(1-ac/a)
V: crack velocity; Cr:Rayleigh Wave speed; C0: dilatational wave speed; a: crack length; ac:initial critical crack length.
If you set crack length "a" to infinity, you can find the crack velocity limits as
Mott: V ->0.38*C0
Freund: V->Cr
Therefore, from Freund's model, the crack velocity is limited by Rayleigh Wave speed. This is what you said.
However, from Mott's model, the crack velocity V is limited by 0.38C0. More test data support Mott's model though, it is the oldest one.
Some other models were also proposed. Recently, Prof. W Yang (Tsinghua University, China) and Prof. H Gao (Plant Max, Germany) did predictions that the crack velocity can exceed Cr. Prof. Rosakis (Caltech, USA) confirmed this throuth tests. If you have further interests, you may consult them.
In brief, the statement of "crack velocity is limited by Rayleigh wave speed" is a math model prediction based on energy balance.
2. and if in kinking case, why are we not apply this method (VCCT)?
The popular VCCT works for selfsimilar cracks. In other words, crack must extend along its original orietation. For kinking, the crack suddenly changes its direction, and a modified version of VCCT is needed. Some detailed discussions can be found in my papers, particularly the first one:
1. Xie D, Waas AM, Shahwan KW, Schroeder JA and Boeman RG, Computation of strain energy release rate for kinking cracks based on virtual crack closure technique, CMES: Computer Modeling in Engineering & Sciences, 6(2004): 515-524.
2. Xie D, Waas AM, Shahwan KW Schroeder JA, and Boeman RG, Fracture criteria for kinking cracks in triple material bonded joints, Engineering Fracture Mechanics, 72(2005): 2487-2504. (Science Direct Top 25 Hottest Articles, #3, Jul-Sep, 2005, #13, Oct-Dec, 2005)
3. And final, I have not yet understood in your sample in the paper "Analysis of mixed-mode dynamic crack propagation by interface element based on virtual crack closure technique" because if with that initial crack direction, loading and constraints, I think the direction of crack propagation will straight (perpendicular to the right line of the plate). Would you please explain to me some my above wonderings.Thank you very much.
Your thinking is absolutely right. Actually, the test observations support your saying. This is because that cracks always like to propagate in pure mode I locally.
In this example, the crack was forced to grow along a predefined crack path so that make it mixed-mode. In reality when you test it, it may not propagate that way. I chose this example because it was simulated by Profs. Atluri and Nishioka by using their moving singular elements and thus I was able to verify my UEL implementation. And also want to see if this kind of problems can be simulated in a much simpler way.
In brief, this is just simply a math example to verify codeing.
Hopefully my answers could be some kind of help to you.
Good luck!
De
Thank you very much Prof. Xie De
Thanks a lot for your comments and i will read them. I hope I will get new knowledge from them. Again thanks.
Chau
I have similar problems
Dear all,
I have similar problem with Chau. I am able to get the stress intensity factor for static loading, but for transient, I was unable to get my stress intensity factor with respect to time using POST26.
Pls advise. Thank You
Dynamic Stress Intensity Factor
I wanted to get some insight in the transient stress intensity factor (SIF).
In the time history, we notice there is an overshoot (~27%) from the
steady state SIF for a fixed (not propagating crack). I found the
overshoot occurs at the time when the reflected wave from the opposite
crack-tip comes back to the first crack tip. I wanted to know why this
overshoot occurs, what is the physical explanation?
Sandip Haldar
Can't get ansys to list the results
Hi,
I also have this problem of getting ANSYS to list the results of the stress intensity factors against time,i was wondering whether could anyway give me some tips on how to progress. I am really stuck in a rut. Please help. Your help will be very much appreciated. Thank you.
crack is open due to loading in the beam in ansys
pls tell me the stepwise procedure to create crack in the beam and also crack open and close in the cantilever beam in ansys mechanical apdl..how u write alogorithm in ansys window to run a program as soon as possible..in my email-swagatmahata.337@gmail.com