September 16, 2020 at 5:28 pmDave LoomanAnsys EmployeeIn the input below the POST26 RESP command is used to compute the shock response spectrum for a 20g triangular acceleration of 10 milli-sec duration. The time-history includes time after the shock load for the lower frequencies to reach their peak displacement value. The input assumes that a modal analysis has been done and expanded.n! After a modal analysis...npi=acos(-1)namplitude=20 ! pulse amplitude (20 g)nwidth=0.01 ! pulse width (10 milli-secs)n n*dim,acel,table,4,1nacel(1,0)=0.0, 0.5*width, width, 5.0*widthnacel(1,1)=0.0, amplitude, 0.0, 0.0n n/axlab,x,TIME n/axlab,y,ACEL (g)n*vplot,acel(1,0),acel(1,1) ! verify acceleration inputnThe table array, acel, can now be used as input to the RESP command in the time-history post-processor.n/post26nstore,alloc,10 ! allocate the number of frequencies to be solved fornvput,acel(1,0),1,0 ! variable 1 is time valuesnvput,acel(1,1),2,0 ! variable 2 is acceleration valuesndata,5,1,10,1,Frequncy ! variable 5 is frequency list (I love this old command!) n(10F5.1)n10.0 20.0 30.0 40.0 50.0 60.0 70.0 80.0 90.0 100.0n n! Use parameters for RESP command input to make more readablenSpec=6 ! variable to contain spectrum outputnFreq=5 ! variable with frequencies to be solved fornInp_Acel=2 ! variable with acceleration inputnOut_Type=3 ! create acceleration spectrumnDamp=0.05 ! damping (ratio to critical) to be usednTinc=0.0005 ! integration time step, 20 pts per cycle at 100 hznInp_Type=1 ! acceleration input, new at 14.0n nresp,Spec,Freq,Inp_Acel,Out_Type,Damp,Tinc,,,Inp_Type n n/title,Response Spectrum for %amplitude%g, %width*1000% m-sec shock load (5% Damping)n/axlab,x,Frequency (Hz)n/axlab,y,Peak Acceleration (g)nxvar,Freq ! x axis is frequencynplvar,Spec ! plot acceleration spectrumn n
September 25, 2020 at 2:13 amKarthik RAdministratorThanks for sharing this information. This is very useful.nKarthikn
- 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.
- 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
© 2022 Copyright ANSYS, Inc. All rights reserved.