August 29, 2018 at 3:43 pmAchilleasMilSubscriber
I want to plot the Interlaminar Shear Stresses in a composite plate (by using ACP), but cannot find a proper documentation or tutorial.
Are there any tutorials on interlaminar stresses? Which shear stresses excactly can ANSYS compute?
In the solution part in Mechanical of the Static Structural Tab I can only request a shear stress plot based on the planes, but I don't know if that is for interlaminar shear stresses or for laminar stresses.
In the ACP Post I have seen there is the ability to choose between σ_ij , where i,j = 1,2,3 and the ability to click on interlaminar normal stresses, but for interlaminar I haven't found anything.
In order to compute those stresses do I have to use only solid elements or can I also use shell elements safely?
Can you help me?
August 29, 2018 at 6:46 pmSandeep MedikondaAnsys Employee
According to manual, here is what we have on the Interlaminar stress:
In the analysis of layered composite structures, shell elements are widely used to keep the computational effort reasonable. In-plane stresses and even transverse shear stresses can be predicted with accuracy using shells based on the first-order shear deformation theory (FSDT). However, in the analysis of thick-walled curved structures, interlaminar normal stresses (INS) can play a significant role. The normal stresses may affect the failure mode or even cause delamination failure. INS computation is not commonly available in shell element formulations, which leads to use of computationally expensive solid modeling instead.
The approach by Roos et al. for INS computation of doubly curved laminate structures represents an alternative for solid modeling. The basis for the INS calculation is the displacement solution obtained from a shell based model. In conjunction with the INS approach, transverse shear stresses are computed with the approach presented by Rohwer and Rolfes. When considered at layer interfaces, transverse shear stresses are referred to as interlaminar shear stresses (ISS).
R. Roos, G. Kress, and P. Ermanni. A post-processing method for interlaminar normal stresses in doubly curved laminates. Journal of Composite Structures. Vol. 81. pp. 463-470. 2007.
K. Rohwer. Improved Transverse Shear Stiffnesses for Layered Finite Elements. DFVLR-FB. 1988.
R. Rolfes and K. Rohwer. Improved Transverse Shear Stresses in Composite Finite Elements Based on First Order Shear Deformation Theory. Int. J. for Num. Meth. in Eng. Vol. 40. pp. 51-60. 1997.
In this part of the manual, there are 4 examples with step by step instructions. In the first 2, you can compare Composite Shell against a Composite Solid. Please check those out.
Also, please take a look at the Limitations and recommendations listed here for Interlaminar normal stress calculation.
There are also a few videos on the ANSYS TechTips Channel on ACP. Please check them out and see if it helps:
Hope this helps.
September 5, 2018 at 6:08 pmAchilleasMilSubscriber
Dear Sandeep Medikonda,
I had already seen the theory stated in the manual/documentation of ansys. So I saw there was the ability to compute ISS also in shell elements.
Your links for the examples showed the setup of the correct workflow of how to export shell data or solid data so I managed to run simulations with both.
, but didn't mention which was more accurate on ISS or generally the characteristics of each one.
The only information I could find about what is different in the computation of ISS in those two types, was stated in the limitations and recommendations:
Interlaminar shear strains of linear triangular shell elements can not be evaluated. Interlaminar shear stresses of linear triangular shell elements can be evaluated by ANSYS but not by ACP. By default, the ANSYS .RST results file contains stress and strain data, however, they may be excluded. In the case of excluded stresses and strains, ACP can evaluate stresses and strains on the basis of the deformation and rotation fields in the results file. Nonlinear effects are not considered by ACP and can induce inaccurate stresses and strains. In general, it is recommended to include the stress and strain data in the .RST data. More information can be found in Solutions.
ACP provides a unique method to evaluate interlaminar normal stresses (INS) for shell elements. This calculation of the INS requires the evaluation of the shell curvature. It is therefore recommended to use quadratic shell elements when INS are of interest. The quadratic elements contain the curvature information per element and offer a better approximation than linear elements. The curvature for a linear shell element is determined from its neighboring elements. This evaluation does not consider INS induced by edge effects or out-of-plane loads (e.g. inserts, pressures, etc.).
But still here it is not clear what is better to use, shells or solids? ( My model has no curvature )..I managed to get similar results (in ACP Post) with solid data and shell data in ISS, after the recomputation which is offered for solid models in ACP Post, but it is different from the values stated in the results of Mechanical for each ply and for the wole layup. So Mechanical results for shells, Mechanical Results for solids and ACP Post results are three diferent things.
Can you help me with that?
September 5, 2018 at 9:27 pmSean HarveyAnsys Employee
I see your concerns. Here are some recommendations which may overlap with what you already have read, but for completeness sake, I will include them here.
1. Include the stress and strain data on the rst. This is pretty straightforward.
2. Mechanical and ACP have stresses reported differently. ACP reports in the fiber/matrix and results are a single value per element. Mechanical can report in the Global or local or Fiber/matrix and you will get the distribution based on the gauss point result variation, hence not a single value. Be careful in how you are comparing. I recommend a simple short beam shear specimen (like 3 point bending) and you can compare with theoretical hand You should see very close agreement between hand calc, shell and solid in ACP and Mechanical, provided the stress gradient is not an issue and you have the proper mesh resolution. This is an exercise I would not skip so you know you are looking at the right quantities in the right way as your baseline.
3. If there are large variations in the material properties, the most accurate ISS will come from modeling each ply as a layer with solid elements. For sandwich construction I would recommend at least a different element for the facesheets versus the core and if the core is thick, I would tend towards solids.
4. The ability to compute INS for shells is a nice feature and won't match exactly but depending on the size of your model as you may not want to model with solids for computational reasons.
5. The recompute iSS is a nice feature to smooth out the ISS and looks closer to theoretical results, but it does assume the shear force on the surface is zero so if your composite body does not have free surfaces, use caution and don't use it.
I hope this helps. Thank you!
September 5, 2018 at 9:35 pmSean HarveyAnsys Employee
One added item. The ISS in composites can have some very high gradients (singular) at free edges and this can be seen by diving into the equilibrium equation. The mesh needed is tiny to often see this phenomenon, just as a note - you may not be interested in edge effects. Some colleagues have put together this nice article which you should refer to on the topic of ISS in composites.
- 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.
- 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
© 2023 Copyright ANSYS, Inc. All rights reserved.