September 15, 2020 at 6:40 pmdj_45516SubscriberHi I am performing a static structural analysis on a simple curved beam. I'm applying a Load on a specific node which is on the tip of the beam. The load I am applying is using APDL command language which is given below. I am trying to retrieve the displacement of this node for all the load steps and the corresponding load steps also in a output text file or anywhere explicitly as result.n/SOLU ! Enter the SOLUTION processornANTYPE,STATIC ! Static (steady-state) analysisnKBC,0 ! Apply load in steps, not rampnSNODE=745 ! Start node index in blade tipnNSEL,S,,,SNODE ! Select nodesnF,ALL,FY,-10. ! Force in y-directionnOUTPR,NSOL,1nOUTRES,NSOL,1 ! Write node solutions to the result filenOUTPR,NLOAD,1nOUTRES,NLOAD,1 ! Write forces to the result filenNSUBST,10 ! Number of substeps for forcenSOLVEnSAVEnFINISH nI believe this should be straight forward and I'm making it quite complicated. The APDL command writes it into the result file but I want it in a text file. nI have no prior ANSYS experience, this is the first time working with ANSYS so all the help would be greatly appreciated.nThanks!
September 17, 2020 at 9:22 amCatilinaSubscriberHello,nIf I understood well you just want to retrieve the node displacement with the associated LS in a formatted list in text format ?nYou can create a 2-column array in which you store the substep number in the first column and the value of the displacement in the second, by using *get command (*get,disp,node,snode,u,y or disp=uy(snode)) and looping through every substep.nAfter you write this array in a txt file with the *vwrite command.nHoping it helps you.nn
September 24, 2020 at 4:40 pmdj_45516SubscriberHi @Catilina, thank you for the instructions. I wrote the following code based on the instructions provided: n/post1nset,LIST,2nSNODE = 745n*dim,disp,array,10,1n*cfopen,'myfile','txt'n*DO,i,1,10,1n*get,disp(1),NODE,SNODE,U,Yn*ENDDOn*vwrite,disp(1)n(F9.4)n*cfclosenBut I am not getting the result I am expecting. It does generate a text file 'myfile', but inside it is just zeros and nothing else.nArrayI've attached the text file to show how it looks like. n
September 25, 2020 at 12:14 amMike RifeAnsys EmployeeHi - first on the solution set up node 745 is selected, but then the whole model is not selected (allsel) prior to issuing the solve command. Was that the entire command listing? nThen in the post processing the set command is reading the results from the result file. In the *do loop the results are not updated via the set command, so it is *get(ing) the same data 10 times.nn
September 27, 2020 at 12:18 pmCatilinaSubscriberHi, nmrife is right. If you posted the whole command listing you forgot to reselect all the entities prior solving but I suppose you did it otherwise you may have had an insufficient constraint model error.nBesides, as I said, you have to loop through every substep if you want to get the correct results and you must specify the iterator as an index of your array. Here you overwrite ten times the same value on the first index of disp(). So your do-loop should looks like this ;n*do,i,1,10nset,1,i ! retrieves the data set for substep in*get,dispy,NODE,SNODE,U,Y !I prefer not to get the value directly in the array because I had some problems with that back in timesndisp(i,1)=dispy n*enddon*cfopen,'myfile','txt'n*vwrite,disp(1,1) !writes all the lines of the array disp() from the first linen(F9.4)n*cfclosenn
- 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.