fatigue crack growth in APDL (XFEM method)

  • 495 Views
  • Last Post 26 September 2018
sohrab posted this 18 September 2018

Hi everyone,

I am trying to model and simulate fatigue crack propagation using XFEM method in APDL.

Order By: Standard | Newest | Votes
sohrab posted this 18 September 2018

 

 

 

Following is the meshed model prepared for XFEM analysis

 

 

 

 

 

1.      1, İs it required to define local coordinate system at crack tip in XFEM method?

 

2.      2, Even in SING method I cannot define my crack tip inside an element, why?

 

3.       In order to constant amplitude loading I follow the following ,

 

time, 1.0

 

deltim, 0.02, 0.02,0.02

 

while

 

CGROW, FCG, METH, LC  ! life-cycle method

 

CGROW, FCG, SRAT, 0 ! stress-ratio

 

!loading frequency is 25 Hz

 

 

 

 

 

3,Does the abovementioned strategy true?

 

4.       4,How I can monitor cycle by cycle crack propagation and related crack parameters (a, deltaK and N)?

 

5.     5,  Crack front node number mentioned here does not listed in APDL node list call; is this a virtual node produced fro XFEM?

 

6.       6,By changing the loading magnitude and frequency I always get the following graphic. There is no change in the amount of crack growth (graphically).

 

 

 your helps and comments to help me fınd out my answers are fully appreciated in advance

 

 

SandeepMedikonda posted this 19 September 2018

Hi Sohrab,

1.      1, İs it required to define local coordinate system at crack tip in XFEM method?

It is usually helpful, but it is not required if the crack is aligned with the global cartesian system.

2.      2, Even in SING method I cannot define my crack tip inside an element, why?

The singularity method allows a crack to terminate within an element, but the original crack tip must be located at node.

 

DoeDoes the above mentioned strategy true?

It looks OK

How I can monitor cycle by cycle crack propagation and related crack parameters (a, deltaK and N)?

You need to use *GET to obtain those values (see example 3.5.5 in the MAPDL Fracture Analysis Guide

Crack front node number mentioned here does not listed in APDL node list call; is this a virtual node produced from XFEM?

yes

By changing the loading magnitude and frequency I always get the following graphic. There is no change in the amount of crack growth (graphically).

 

The graphic results are scaled to be visible. Use /DSCALE to change the scale factor

Regards,

Sandeep

Guidelines for Posting on Student Community

 

  • Liked by
  • sohrab
sohrab posted this 20 September 2018

 

Thank you Sandeep for your Answer. youre reply are so helpful.

 

1, İs it required to define local coordinate system at crack tip in XFEM method?

 

It is usually helpful, but it is not required if the crack is aligned with the global cartesian system.

 

my concern is that, Does XFEM in APDL automatically take care about tip coordinate to calculate SIFs? if not, then how should crack tip coord'nate be defined to follow crack tip during propagation

 

How I can monitor cycle by cycle crack propagation and related crack parameters (a, deltaK and N)?

 

You need to use *GET to obtain those values (see example 3.5.5 in the MAPDL Fracture Analysis Guide

 

in case of crack tip extention Iam not sure how to retrieve crack tip coordinates (as it is a virtual node(in 2D case) ) to measure crack extention at each substep loading.

 

can you help me in this regard?

 

By changing the loading magnitude and frequency I always get the following graphic. There is no change in the amount of crack growth (graphically).

 

The graphic results are scaled to be visible. Use /DSCALE to change the scale factor

 

but it seems that the crack direction also keeps the same.

 

and my last question:

 

how can I stop the loading (simulation) when crack length reaches an specific amount?

Regards,

Sohrab

 

SandeepMedikonda posted this 21 September 2018

Hi Sohrab.

1, İs it required to define local coordinate system at crack tip in XFEM method?

 

It is usually helpful, but it is not required if the crack is aligned with the global cartesian system.

 my concern is that, Does XFEM in APDL automatically take care about tip coordinate to calculate SIFs? if not, then how should crack tip coord'nate be defined to follow crack tip during propagation

 

A:  You define the crack characteristics, including crack coordinate system, using the CINT command.  If you do not explicitly define a crack coordinate system using CINT, the solver assumes that it is global cartesian.

 How I can monitor cycle by cycle crack propagation and related crack parameters (a, deltaK and N)?

 You need to use *GET to obtain those values (see example 3.5.5 in the MAPDL Fracture Analysis Guide

 in case of crack tip extention Iam not sure how to retrieve crack tip coordinates (as it is a virtual node(in 2D case) ) to measure crack extention at each substep loading. can you help me in this regard?

A:  You cannot *get the “new” crack tip coordinates.  You can only obtain the crack extension DLTA. See Example 3.7.5 in the MAPDL Fracture Analysis Guide.

 

By changing the loading magnitude and frequency I always get the following graphic. There is no change in the amount of crack growth (graphically).

The graphic results are scaled to be visible. Use /DSCALE to change the scale factor

but it seems that the crack direction also keeps the same.

A:  The direction should remain constant.

 

and my last question:

how can I stop the loading (simulation) when crack length reaches an specific amount?

A:  There no automated method.  You might be able to monitor the crack progression by placing the solve inside a *DO loop with a *IF statement that either processed the next solve or ended the solution based on some variable.  You might also be able to use the *DOWHILE command. Either approach would require some sophisticated APDL scripting.

Regards,

Sandeep

  • Liked by
  • sohrab
sohrab posted this 26 September 2018

Hi Sandeep

first of all thank you for your comprehensive answer.

I progressed a lot in my problem since last post. but now there seems to be a problem with crack definition in ansys.

1. an element with ID 4642 has 2 crack front which is prohibited

2. an element with ID 4635 is not possible to calculate psi and phi values

I double checked every thing but still it does not work for me.If it is possible for you to take look at it would be great. please just let me know if you can check the code to send you the script.

Regards,

Sohrab

Close