July 23, 2021 at 3:11 pmelhamasadiSubscriber
Trying to simulate a crack on a 3D curved surface (the attached geometry), I cannot find a way to accurately capture a crack. Can anyone please give me some instructions on this issue?July 23, 2021 at 10:25 pmJuly 24, 2021 at 3:34 amelhamasadiSubscriberI want to draw
(1) an edge crack (length= 100 mm, gap=10 mm), in the middle of one of the edges
(2) a crack at the center (the same dimensions)
Provided that I need the geometry to remain as surface body, so that I can apply simply supports on four edges later on in mechanical environment
July 24, 2021 at 12:07 pmpeteroznewmanSubscriberIn SpaceClaim, create an XY plane by clicking on the Z axis. Select that plane and start a Sketch. Use the construction line tool to draw a 100 mm line at the center of the plate. draw a 5 mm construction line from the center of that first line 90 degrees to it on one side. Repeat for the other side. Select the 3 point curve tool. Click on one end of the 100 mm line, then the other end, then the 5 mm end. Repeat for the other side. Exit the Sketch. Use the Project button. Select the two curves, then your curved surface. Finally, delete the surface created by the Project and you have a crack.
July 24, 2021 at 3:55 pmelhamasadiSubscriberThank you for this detailed demonstration. But I meant crack modelling in the mechanical environment using pre-meshed crack, arbitrary crack or semi-elliptical one. Because I keep receiving this error:
One of the crack's mesh encompasses multiple bodies which have different material models. Ensure one material model by scoping these bodies to one material assignment object.
July 24, 2021 at 5:34 pmpeteroznewmanSubscriberTo use the Fracture tool, you need solid elements. You can't use the Fracture tool on shell elements.
July 24, 2021 at 7:40 pmJuly 26, 2021 at 10:20 amelhamasadiSubscriberSo as you mentioned, I've tried to model the geometry as a solid geometry (using pull option in Spaceclaim), but I still cannot capture the crack using semi-elliptical (Tetrahedron mesh), pre-meshed or arbitrary crack. The message I receive here is that the mesher fails to generate mesh.
Here are my applied settings in semi-elliptical method:
July 26, 2021 at 12:43 pmpeteroznewmanSubscriberCracks can only be created on Quadratic Tetrahedral elements. Did you set the Mesh to Quadratic?
Automatically meshed Semi-Elliptical cracks must remain in the solid body. The minor radius is 10 mm and the largest contour radius is 10 mm so the part must be at least 20 mm thick for the mesher to work. I don't think your geometry is more than 20 mm thick is it? You also need a base mesh that has many elements covering that 20 mm depth.
See my reply in this discussion: https://forum.ansys.com/discussion/comment/126047#Comment_126047
January 12, 2022 at 11:29 amaceloraSubscriberHi, i have a similar question. I want to simulate 2 cracks on a composite that consist of 2 materials.
The first crack location is along the interface while the second is near the interface and near the first crack location.
how do i draw the crack such that it is along the interface?
I will also need to make 2 different interface. One straight line interface and the other is wavy
January 12, 2022 at 12:32 pmpeteroznewmanSubscriberI assume you are using solid elements to mesh the two materials.
Let's say you have a material called fiber, which has a rod shape that exists in a material called epoxy.
A model of the composite would have a solid block of epoxy with rod-shaped holes in it, and rods would fill those rod-shaped holes with fiber material.
For that model to have no crack, you would use shared topology to cause the mesh of one material to be connected by shared nodes to the next material.
But maybe you have a material called coating on the surface of a material called substrate.
You do the same thing with shared topology to make a composite material with no cracks.
What you need to do to introduce a crack at the interface is to split the faces on each material at the interface. When you do shared topology, you exclude the faces where you want the crack and include the faces where you don't want a crack.
If you want more detailed instructions, you will need to provide a far more detailed description of your geometry with a lot of images inserted into your reply to show what you are trying to do.
January 13, 2022 at 12:19 pmaceloraSubscriberThank you for your reply, as of now the geometry,material, location of crack and crack size is left entirely up to individual or rather me.
How do i change the interface to straight line or wavy though?
January 13, 2022 at 12:54 pmpeteroznewmanSubscriberTo make a wavy crack, draw a wavy curve (spline) extrude that into a surface, use that surface to cut the faces of the materials.
As I said, if you want more detail, reply with an image of what you want.
March 8, 2022 at 6:14 amaceloraSubscriberHi currently this is all i have, i created a 100 x 100 x100mm cuboid with the top half being stainless steel and bottom half being inconel 718.
Below is what i need to do for the interface a wavy and straight line. It is not a wavy crack that is required of me.
Currently how do i go about changing the interface to wavy and creating 2 cracks near the interface?
March 8, 2022 at 1:17 pmpeteroznewmanSubscriberTo make a wavy interface, draw a wavy curve (spline) extrude that into a surface, use that surface to cut the cube. In SpaceClaim, use the Share button on the Workbench tab to connect the meshes of each half.
In ANSYS Help are several tutorials on how to create a crack.
March 8, 2022 at 2:44 pmaceloraSubscriberHi Peter, thank you for your advise, however i am required to create the crack near the interface in this case. is there any difference in this case?
March 9, 2022 at 1:22 ampeteroznewmanSubscriberJust make sure the solid elements are small enough near the interface before you add a crack near the interface. Make sure there are at least 10 elements between the crack and the interface.
March 12, 2022 at 5:44 amMarch 12, 2022 at 11:48 ampeteroznewmanSubscriberIn the outline, select the two Solid bodies, right click and select Form New Part. Now the two bodies will have a connected mesh across the interface. This is called Shared Topology.
November 25, 2022 at 8:03 pmMEHDI BENJSubscriber
I'm trying to create a crack on an imported winglet geometry. What are the steps to take to create a crack. I'm assigned to simulate ultrasonic propagation on composite winglet in healthy state and unhealthy state(crack). Thank you for your time and hope you have a good day.December 6, 2022 at 4:08 ammine_mewSubscriberDecember 6, 2022 at 4:11 ammine_mewSubscriber
I am trying to create delamination on a composite blade. This blade is surface geometry and is assembled with many parts but the considered section is the top surface (I want to create the delamination on this part).
I am confused as below;
- To create delamination, the blade geometry should be solid elements.
- The geometry imported to ACP should be the surface type but the ACP can generate to solid element by the "solid model" command. So I don't know how to create delamination after setting parameters in ACP
- I assign the composite stack in ACP (e.g. 0/90/90/0). If I want to create delaminate between 0 and 90. How can I do it?
Could you please suggest me how to create delamination on the composite blade (curve surface)?
Thank you in advance
PanidaViewing 21 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.