Tagged: userdefinedresults


December 13, 2022 at 4:21 pmMarco CastelliSubscriber
Hi,
I solved a static structural analysis neglecting non linear material effects. Than I duplicate that analysis (same materials, geometry, mesh and BC) and solved it considering also non linear material effects. Materials are modelled as Multilinear Isotropic Hardening but, the first analysis manages materials as perfectelastic, the second one considers also plasticity.
Now I'd like to use an User Defined Result which sums S1 of the elastic FEA plus S1 of the elasticplastic FEA but I don't know how to do that.
Thanks in advance.
Marco

December 13, 2022 at 7:18 pmpeteroznewmanSubscriber
Why do you want to sum the Max Principal stress from two copies of the model? You will get double the stress.
A common workflow is to have one linear model with two or three orthogonal loads where the model takes a long time to solve. An example is a 1G acceleration load that is applied in the X, Y and Z direction, one load in each of three copies of the Static Structural model. Then results for an acceleration load in any direction of any magnitude can be quickly created using Solution Combinations.
In Mechanical, right click on the Model branch of the Outline and Insert a Solution Combination. Then linear combinations of the three load cases can be calcuated from the solutions of the unit load cases without needing to solve again, so these results are available immediately.

December 14, 2022 at 9:23 amErik KostsonAnsys Employee
Hi
Not sure why you do this (also be careful if it is used for something important, say design of structure), but here goes.
The only way of doing this is.
 Have one model with 3 steps.
 Define one kin. plasticity or bilinear iso. plasticity material. Set it with very high yield so it is basically used as the linear material as it will never yield.
 Define 3 steps. 1^{st} step uses the material mentioned above with load, 2nd step goes back to unloaded, and 3rd nonlinear material step with load again.
 In the 3rd step change the material properties to the real plastic ones and not the very high ones used in step 1. This is done via command snippet (placed in the Solution tree) that is only active in step 3 (set step selection mode to number and enter below it step number 3). The nonlinear material shown below needs to be of the same sort of plasticity as in the material used in step 1 (so the one defined in engineering data)!
!change the below as needed for your own properties (they need to have the same plasticity so both need to be bilinear iso. Hardening plasticity here)
MP,DENS,2,7850, ! kg m^3
MP,EX,2,200000000000, ! Pa
MP,NUXY,2,0.3,
TB,PLAS,2,1,,BISO
TBTEMP,22
TBDATA,1,200000000,10000000000
MPCHG,2,ALL Use solution combination to combine the results from step 1 (linear) and step 3 (nonlinear material).

December 14, 2022 at 10:51 amMarco CastelliSubscriber
Dear peteroznewman and Erik Kostson,
Thanks for your answers.
answer to peteroznewman:
"Why do you want to sum the Max Principal stress from two copies of the model? You will get double the stress."
Actually I do not sum Max Principal stress, it was just to make the easiest example. I am performing a fatigue analysis and ASME asks to compare strains from elasticplastic analysis and from elastic analysis.
answer to Erik Kostson:
I did not kwnow that I can performe a single analysis modifing material propoerties along the time steps. Unfortunatelly I never used ADPL so this solution is quite complex for my ability because I have several materials in the same model. Maybe if I could deactivate/activate the comand for Nonlinear effect of the material along the time steps, it would be easiest.
Is that possible? Could you please help me to write the adpl code?
Regards,
Marco

December 14, 2022 at 10:58 amErik KostsonAnsys Employee
Hi
I can not help with that, but what I would suggest is that you look up and understand the commands I posted and use them as needed – aslo reading up on apdl and the apdl command reference (e.g., MPCHG command etc) is good if you want to use that in the future (apdl commands in mechanical).
Also you can just have two different models (one linear and the other nonlin.)  export results to excel from both, and then combine them as you want – all the best
Erik

 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.
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.
 Saving & sharing of Working project files in .wbpz format
 Understanding Force Convergence Solution Output
 An Unknown error occurred during solution. Check the Solver Output…..
 Solver Pivot Warning in Beam Element Model
 Colors and Mesh Display
 whether have the difference between using contact and target bodies
 How to calculate the residual stress on a coating by Vickers indentation?
 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

2688

2130

1349

1136

461
© 2023 Copyright ANSYS, Inc. All rights reserved.