

March 2, 2023 at 1:12 amlongt8Subscriber
Hello Ansys Support Team,
I am trying to find the J integral for mix mode. I have an example for mixed mode 1 and 2. When I select the crack opening direction as Y (0,1,0), it should be Mode 1. Would you let me know is it correct for me to get Mode 2 J integral value by checking the crack open direction as X (1,0,0)? We can see the J integral values for Y (0,1,0) and X (1,0,0) are not the same. Also, would you let me know how can I get the mix mode J integral for this example?
Thank you so much!
Teng

March 7, 2023 at 8:19 pmAndreas KoutrasAnsys Employee
Hello,
Please let us know if the following are of any help:
https://www.dynamore.de/de/download/papers/2015lsdynaeurop/documents/sessionse58/nonlinearfracturemechanicsinlsdynaandlsprepost/view
Jintegral in 3D: https://www2.dynamore.se/public/jernberg/jintegral.gif
Jintegral in 2D: https://www2.dynamore.se/public/jernberg/jintegral2.gif
LSPP Help > DocumentationThanks

March 8, 2023 at 2:14 amlongt8Subscriber
Hello,
Thank you so much for your reply. In the two video toturals, I notice the boundary is applied in Y direction. Thus the "Crack opening direction" is seleced as Y (0,1,0). Thus the two video tuturals are desinged for mode 1.
I have tried to downloade the docuemnt several times, but the document contens is empty:
Would let me know how I can let this docuement works?
I am really appreciate if you would let me know how I can do J integal for mix mode. Is that simpily change the crack opening direction vector? If the nodal displacement around crack is 1 in X and 10 in Y, then the crack opening diection should be (1,10,0) to compute the mix mode 1 and mode 2?
Thank you so much!
Best,
Teng

March 9, 2023 at 7:03 pmAndreas KoutrasAnsys Employee
Hello Teng,
The LSPP developer shared the following comment:
Interesting question.
I think this is due to a confusion regarding the stress intensity factors K_{I} K_{II} K_{III} from
Linear Elastic Fracture Mechanics (LEFM), and the J – integral from nonlinear fracture mechanics.
The J integral is an energy measure, related to the energy released for an infinitesimal increase in
crack length. It will consider all loading modes (opening, shearing, twisting) “lumped” so to say.
It will consider mixed mode loading, but it will not be possible to distinguish between the modes.
If the material response is elastic, the stress intensity factors and the J – integral value will be
related byThe implementation in LSPrePost assumes a traction free crack surface. So, if a contact
between the crack faces is defined and active (crack closure or shearing with friction) the
results from LSPrePost will not be entirely correct. From the images, this does not seem to be
the case though.
In LSPrePost, the two points (crack tip node, crack surface node) and the normal to the
crack surface (Crack opening direction) will define a local Cartesian coordinate system
with the origin at the crack tip and the xaxis along the crack surface. This coordinate system
is used for evaluating the J – integral for cracks with arbitrary orientation. The infinitesimal
crack length increase is assumed to occur along the local x – direction.
So in the images, the Crack opening direction must be (0, 1, 0) and it does not depend on the
loading, only the geometry. If the Crack opening direction is input as (1, 0, 0) incorrect results
will be obtained (as indicated by the negative J – values in the image).I hope this helps.

March 9, 2023 at 7:08 pmAndreas KoutrasAnsys Employee
Regarding the documentation:
You can get both documentation and tutorials by going to Help in LSPrePost and click on Documentation and Tutorial, respectively. First time you click on it, LSPrePost will have to download the files but afterwards they are ready to use without downloading again.
After these files are downloaded, they need to be placed in the "resource/HelpDocument" subdirectory beneath the LSPP executable location.

March 12, 2023 at 12:54 amlongt8Subscriber
Hello Andreas,
Thank you so much for your reply in detail and I really appreciate it! I can read the LSPP help docuement now.
However, I still have questions for J integtal in LSPP which confused me for long time. In the figure below, the left one is designed for Mode1 J integral and right one is designed for mode 2 J integal. The left one which is for Mode 1 has loading in position Y direction on the top and the total fixed boundary on the bottom. The right one which is for Mode 2 has loading in position X direction on the top and the total fixed boundary on the bottom.
Would you let me know if the crack opening direction vector for both case is (0,1,0) or (sin theta, cos theta,0)?
The vector (sin theta, cos theta,0) seem make more sense and agree with the docuement, but toturals(https://www2.dynamore.se/public/jernberg/jintegral.gif and www2.dynamore.se/public/jernberg/jintegral2.gif )above use (0,1,0) for not perfect crack example
Thank you so much!
Best,
Teng

March 16, 2023 at 7:13 pmAndreas KoutrasAnsys Employee
Hello,
In the previous reply, the developer had explained:
"The J integral is an energy measure, related to the energy released for an infinitesimal increase in crack length. It will consider all loading modes (opening, shearing, twisting) “lumped” so to say. It will consider mixed mode loading, but it will not be possible to distinguish between the modes ...
The infinitesimal crack length increase is assumed to occur along the local x – direction. So in the images, the Crack opening direction must be (0, 1, 0) and it does not depend on the loading, only the geometry. "
I believe this should answer your question.

 You must be logged in to reply to this topic.
Boost Ansys Fluent Simulations with AWS
Computational Fluid Dynamics (CFD) helps engineers design products in which the flow of fluid components is a significant challenge. These different use cases often require large complex models to solve on a traditional workstation. Click here to join this event to learn how to leverage Ansys Fluids on the cloud, thanks to Ansys Gateway powered by AWS.
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.
 explicit dynamics
 Explicit dynamics ERRORS
 turning simulation
 getting zero maximum and minimum stress value in explicit analysis
 How do get Full values instead of just minimum and maximum ?
 How to figure out impact force in Explicit Dynamic Analysis
 Monte Carlo Simulation
 Euler Domain Restricting Simulation
 Running an explicit dynamics simulation on a composite plate
 Which analysis to use for dynamic and quasistatic compression of auxetic structures?

3778

2587

1831

1242

598
© 2023 Copyright ANSYS, Inc. All rights reserved.