October 9, 2023 at 9:00 amaecm20Subscriber
I have a study with multiple loads applied in individual static structural systems. For bolt analysis I want to get the reaction force across a contact. I am using the solution combination tool to combine the loads into various load cases. Using 2021 R2.
The problem I have is that the colution combination tool doesnt have a force reaction result option. I can set the geometry to a surface and use the user defined result tool with ENFOX, Y or Z to get the elemental nodal forces. If I export and sum these (for each node) I get the right output, but only at one solution combination. I have 26 load cases and 12 surfaces though so doing this process manually is not practical.
Is there a way to sum the elemental nodal forces within the expression line so it gives a total force maximum instead of the macimum nodal force.
Things I have tried; sum, identifiers, ENFOVECTORS, submodelling.
Maybe this is within the user manual but I cant see it anywhere.
All help much appriciated.
October 11, 2023 at 4:25 ammjmiddleAnsys Employee
Solution combination and Design Assessment will not allow probes. A “DA Result” under a “Design Assessment” system has a “Sum Results” that should do what a force probe result would, but it is unsupported, and I can’t get the DA Result to work for anything anymore.
You would need to use scripting by some means. Either script in Mechanical or APDL:
Run script in Mechanical in “Automation > Scripting”:
# First create force probe under each analysis containing the text "for_combination"
# Then run the script below
sumResultX = None
sumResultY = None
sumResultZ = None
for analysis in ExtAPI.DataModel.Project.Model.Analyses:
# Solution Combination is limited to static structural systems, so lets do that too
if analysis.AnalysisType == AnalysisType.Static:
probes = [result for result in analysis.Solution.Children if "for_combination" in result.Name]
if len(probes) > 0:
probe = probes # use 1st one
if sumResultX == None:
sumResultX = probe.XAxis
sumResultX += probe.XAxis
if sumResultY == None:
sumResultY = probe.YAxis
sumResultY += probe.YAxis
if sumResultZ == None:
sumResultZ = probe.ZAxis
sumResultZ += probe.ZAxis
print("X Axis: " + str(sumResultX))
print("Y Axis: " + str(sumResultY))
print("Z Axis: " + str(sumResultZ))
Method 2:Use APDL script. This involves loading results of each analysis and then using load case commands. Generally:/post1
file,file1,rst ! Start with first results file
set,1,1 ! Read into memory load step 1 substep 1
file,file2,rst ! Switch to second results file
lcdef,1,1,1 ! Assumes 2nd result is load step 1 substep 1
!insert any lcfact commands
lcoper,add,1 ! Add results together
reswrite,file ! use new file name since it can append to a pre-existing results file.
Load results in Mechancial and view there using “Tools > Read Results Files…”
Make sure you select the correct units the solution was ran in.
You may get an error, “An unknown error occurred during solution.” But the solution should be correct.
- You must be logged in to reply to this topic.
Boost Ansys Fluent Simulations with AWS
Computational Fluid Dynamics (CFD) helps engineers design products in which the flow of fluid components is a significant challenge. These different use cases often require large complex models to solve on a traditional workstation. Click here to join this event to learn how to leverage Ansys Fluids on the cloud, thanks to Ansys Gateway powered by AWS.
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
- Solver Pivot Warning in Beam Element Model
- Understanding Force Convergence Solution Output
- An Unknown error occurred during solution. Check the Solver Output…..
- 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.
- whether have the difference between using contact and target bodies
- Defining rigid body and contact
- Colors and Mesh Display
- A solver pivot warning or error has been detected
© 2023 Copyright ANSYS, Inc. All rights reserved.