May 16, 2021 at 3:15 pmPuhanSubscriber
I hope you are doing well.
I am having a problem with XFEM while writing APDL in Ansys Workbench.May 18, 2021 at 7:34 amPuhanSubscriberHello
It has been some days and I could not find almost noting in this forum can anyone makes a discussion on this please, this has already been solved in APDL in Ansys manual I am just trying to replicate the same in Workbench as have to solve some other problems.
The whole problem is explained above. It is a three-point test. The below is the whole interface as you can see
The command is written is like following
"!Commands inserted into this file will be executed just prior to the ANSYS SOLVE command.
!These commands may supersede command settings set by Workbench.
!Active UNIT system in Workbench when this object was created:Metric (mm, t, N, s, mV, mA)
!NOTE:Any data that requires units (such as mass) is assumed to be in the consistent solver unit system.
!See Solving Units in the help system for more information.
tb, cgcr, 2, , , STTMAX ! Fracture Behavior: Maximum circumferential stress
tbdata, 1, 0.5 ! Maximum normal traction: = 0.5 N/mm2
!Decay of stresses on newly cracked interface
tb, cgcr, 2, , , RLIN
tbdata, 1, 0.04, , 0.0
! Element component required for XFENRICH command
cm, testcmp, elem
! Define enrichment identification
xfenrich,ENRICH1,TESTCMP ! Defines parameters associated with crack propagation using XFEM
xfdata, ENRICH1, LSM, 939, 1042, 0.047123
xfdata, ENRICH1, LSM, 939, 1043, 0.047123
xfdata, ENRICH1, LSM, 939, 1045, -0.048062
xfdata, ENRICH1, LSM, 939, 1044, -0.048062
/com LISTING OF CRACK INFORMATION
! Crack-tip element
cm, crktipelem, elem ! Element set component for CINT command
! Loading - Displacement on two nodes on top
nsel,s,loc, x, -0.048062, 0.047123
nsel,r,loc, y, 1.5
d, all, uy, -0.16 ! Uy = -0.16mm
d, all, ux, 0
! CINT calculations : Defines parameters associated with fracture parameter calculations
CINT, NEW, 1
CINT, CXFE, crktipelem ! Crack-tip element
CINT, TYPE, STTMAX ! Uses STTMAX
CINT, RSWEEP, 181, -90, 90
! CGROW calculations : Defines crack-growth information
CGROW, NEW, 1
CGROW, CID, 1
CGROW, METHOD, XFEM ! Uses XFEM method for the crack propagation
CGROW, FCOPTION, MTAB, 2 ! Fracture criterion
So kindly please let me know, I will be grateful to you.
Can you sir please look into it? Thank you very much.
May 23, 2021 at 8:36 amPuhanSubscriberSir can you please help? Can we do the same with the command in workbench for XFEM, if no there is an extension I found on the app and I added it in the workbench but I have some questions about that? But can you please at least give the answer to the first question?
I will be grateful to you.
May 26, 2021 at 11:59 pmDavid WeedAnsys Employee
I ran this on my end and discovered the same error regarding the PLANE182 key options. The issue here is that the MAPDL solver has some internal logic by which it forces certain element key options regardless of what you've initially specified. This is done through the ETCON command. You'll see that it's forcing keyopt(1) = 3, which is not supported for XFEM:
ELEMENT TYPE1 IS PLANE182 WITH PLANE STRAIN OPTION. IT IS ASSOCIATED WITH
LINEAR MATERIALS ONLY AND POISSON'S RATIO IS NOT GREATER THAN 0.49. KEYOPT(1)=3
IS SUGGESTED AND HAS BEEN RESET.
To override this, simply use ETCON,OFF in /PREP7. For instance, I place all of the material information in a command object under the surface body and you can see that etcon,off is set first:
with this, the simulation ran to completion.
May 27, 2021 at 7:21 amPuhanSubscriberDear David
Thank you very much, I will try to implement that.
Also, can you please clarify if xfem can be used in Ansys in 3D or not?
Again thank you very much, it will help a lot.
May 27, 2021 at 4:47 pmDavid WeedAnsys Employee
XFEM is supported in 3-D; see the help and Example 3.8: Generating a Center Crack in a 3-D XFEM Model (MESH200 Method): https://ansyshelp.ansys.com/account/secured?returnurl=/Views/Secured/corp/v201/en/ans_frac/Hlp_G_FRACXFEM.html?q=xfem
March 10, 2022 at 10:46 amAli_shSubscriber
I have a problem with the XFEM command in the workbench too.
I am trying to solve the same problem that Puhan mentioned earlier. It is not exactly the same I implemented it on the workbench; however, almost the same dimensions and boundary conditions.
I have attached the data file here too.
I do not have a problem defining enriched elements and specifying the crack tip. There is no error, and I also transferred the model to APDL and checked the elements there.
The problem is that the crack will not propagate in my model, although I defined enriched area and pre-crack elements.
I also tried to run with different radii, and nothing changed (CINT, RADIUS, 0.0005)
here is my xflist data:
DISCONTINUITY DATA ASSOCIATED WITH THIS ENRICHMENT NAME:
I also checked the constrain equations after solution by transferring the model to APDL, and here is the result (CELIST). I do not know why the constraint equations are defined automatically in the enriched area after the solution:
LIST ALL SETS FOR CONSTRAINT EQUATIONS WITH ANYNODES SELECTED
MAXIMUM CONSTRAINT EQUATION NUMBER=1409
Would you please look at the file and help me with that?
March 10, 2022 at 3:50 pmAli_shSubscriberMarch 11, 2022 at 10:11 amAli_shSubscriberHi
It is solved.
I added the following in my commands
Viewing 8 reply threads
Ansys Innovation Space
- You must be logged in to reply to this topic.
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.
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.Trending discussions
- Saving & sharing of Working project files in .wbpz format
- An Unknown error occurred during solution. Check the Solver Output…..
- Understanding Force Convergence Solution Output
- Solver Pivot Warning in Beam Element Model
- Colors and Mesh Display
- How to calculate the residual stress on a coating by Vickers indentation?
- whether have the difference between using contact and target bodies
- What is the difference between bonded contact region and fixed joint
- The solver engine was unable to converge on a solution for the nonlinear problem as constrained.
- User manual
Top Rated Tags
© 2023 Copyright ANSYS, Inc. All rights reserved.Ansys does not support the usage of unauthorized Ansys software. Please visit www.ansys.com to obtain an official distribution.