June 3, 2021 at 1:01 pmDoodlerDSubscriber
I'm trying to extract averaged internal nodal forces along an entity. They show values that are wrong. What could be the error? I have turned on nodal forces in the analysis settings.June 4, 2021 at 6:42 am1shanAnsys EmployeeI hope you have checked the units. What is the direction and value of force on the bracket? Also, what does the command snippet do? Could you also try FZ (this works only on constraint nodes) instead of ENFOZ and see if anything changes?
June 4, 2021 at 1:34 pmDoodlerDSubscriberThank you.
The units are fine, the command snippet is to activate ENFO, since it is missing in the solver worksheet. The value of forces are as described below. I'm running a set of benchmarks with Ansys after moving from a Nastran environment. I dont think Fz helps. However, I was able to work with the stress tensor and take the longer route. I'm not sure why ENFO does not work in my case.
June 4, 2021 at 1:59 pmErik KostsonAnsys EmployeeHi
I have made a simple example to show how one can do this perhaps - I am used to working with the element-nodal force vectors when designing saying connections so that is the udr I have used as shown below. We can then export the results to excel and sum the element nodal force to obtain the total reaction which -100 N as shown, and is as expected equal and opposite to the applied load which is 100 N in this example. I think as shown it can be done also with ENFOY.
Should be said here, that mesh is fully compatible at the intersection of the two plates so no contacts - if we have contacts then we can get the reaction at the contact with a contact/force reaction probe (under the force reaction probe we can choose to look at the contact region).
Hope this helps
June 4, 2021 at 2:07 pmDoodlerDSubscriberThank you for looking into it.
What is the 'elemental-nodal' force value? is it nodal or elemental? How is Ansys interpolating this value and where can I read about it. A google search is giving me limited results.
June 4, 2021 at 2:10 pmErik KostsonAnsys EmployeeNo worries - it is the internal forces between elements , so forces within the mesh (so not fixed boundary nodes) which I mean with element nodal force (ENFO)- it is a general term. not sure if it is described. ELement Nodal force is not interpolated as far as I know, they are "raw" and they are the internal forces that provide equilibrium.
Finally in the above example we need to sum (use SUM() function in excel) manually in order to get the total force (ansys provides the force at each node of the element so we need to sum them all)
June 7, 2021 at 3:42 am1shanAnsys EmployeeThanks for working it out !!!
Check this out - 1. Solution Output, 2. Interpolation.
The documentation states that "Interpolation primarily applies to degree of freedom results such as temperatures, displacements, and node-based element results like thermal flux, stress, and strain. Therefore, it is recommended that you not use interpolation for results such as node-based element reactions (EHEAT/ENFO). The application allows for these calculations, but they are not good candidates for interpolation. In addition, you should not sum interpolated results of these types; such as to calculate total heat or total force"
How to access online help ? - https://forum.ansys.com/discussion/22563/using-help-with-links#latest.
Viewing 6 reply threads
Ansys Innovation Space
- You must be logged in to reply to this topic.
Simulation World 2022
Check out more than 70 different sessions now available on demand. Get inspired as you hear from visionary companies, leading researchers and educators from around the globe on a variety of topics from life-saving improvements in healthcare, to bold new realities of space travel. Take a leap of certainty and check out a session today here.
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
- How to calculate the residual stress on a coating by Vickers indentation?
- An Unknown error occurred during solution. Check the Solver Output…..
- Saving & sharing of Working project files in .wbpz format
- Solver Pivot Warning in Beam Element Model
- Understanding Force Convergence Solution Output
- whether have the difference between using contact and target bodies
- Colors and Mesh Display
- The solver engine was unable to converge on a solution for the nonlinear problem as constrained.
- Massive amount of memory (RAM) required for solve
- What is the difference between bonded contact region and fixed joint
Top Rated Tags
© 2022 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.