# MFX FSI: How to apply time-varying load?

 Register Blogs Members List Search Today's Posts Mark Forums Read

 December 16, 2011, 13:18 MFX FSI: How to apply time-varying load? #1 New Member   Join Date: Jan 2011 Posts: 13 Rep Power: 8 Dear all: I'd like to apply time-varying load on structure in a MFX FSI analysis. However, I am very confused about how to set up the procedure in MFX. Currently I guess it's a multiframe restart, but I am not sure. Maybe you can help me. Suppose the load is a time-varying concentrated force to be applied on node 90. The magnitude of the load is: From t=0-1, ramped, force from 0 to 1 From t=1-2, force kept at 1 From t=2-3, stepped, force = 0 From t=3-4, stepped, force = 3 From t=4-5, ramped, from from 3 to 0 Under this situation, What is the corresponding APDL code in the MFX /SOLU part to apply the force on node 90 from t=0 to t=5? Thank you for clarifying my confusion on this issue! Sincerely, Ryan

 December 20, 2011, 11:59 #2 Senior Member   Join Date: Apr 2009 Posts: 532 Rep Power: 14 Are you setting this up in Workbench? If so just set your analysis end time to 5 seconds (this isn't used, but you can't setup the load without this) with 1 loadsteps then apply the force via the Tabular Date option. In the table just start entering the time values with the required force values. To get a step change use two time values that are only 1 time step size apart.

 January 18, 2012, 11:01 #3 New Member   Join Date: Jan 2011 Posts: 13 Rep Power: 8 Thank you for your reply, stumpy. I was away from this problem for a while because of other tasks. I wonder if there are corresponding APDL codes for the task you mention in Workbench? Personally I am more familiar with APDL, and it really speeds up my progress without touching Workbench. Or if it's not a possibility, maybe you can direct me to a Workbench example and I'll start from there. Thank you! Sincerely, Ryan

 January 18, 2012, 15:01 #4 Senior Member   Join Date: Apr 2009 Posts: 532 Rep Power: 14 In the end WB is generating APDL commands, so it's certainly possible in APDL. I don't know the commands, but you could set up a simple example and write out the input file from Workbench, then you can see what commands were used.

 January 19, 2012, 14:48 #5 Senior Member   Edmund Singer P.E. Join Date: Aug 2010 Location: Minneapolis, MN Posts: 512 Rep Power: 13 Create a table parameter in ansys. For example if you are applying force in the x direction in the create a table called xforce: *DIM,xforce,TABLE,7,1,1,TIME, !! !!time in sec !! xforce(0,0,1) =0 xforce(1,0,1) =1 xforce(2,0,1) =2 xforce(3,0,1) =2.0001 xforce(4,0,1) =3 xforce(5,0,1) =3.0001 xforce(6,0,1) =4 xforce(7,0,1) =5 !! !!force in x direction !! xforce(0,1,1) =0 xforce(1,1,1) =1 xforce(2,1,1) =1 xforce(3,1,1) =0 xforce(4,1,1) =0 xforce(5,1,1) =3 xforce(6,1,1) =3 xforce(7,1,1) =0 !! kbc,0 The above will always ramp the loads. We get a step by using a very small time step in the ramp to simulate a step function. Apply the load as follows: f,90,fx,%xforce%

 January 23, 2012, 10:29 #6 New Member   Join Date: Jan 2011 Posts: 13 Rep Power: 8 Dear stumpy and Edmund: Thank you for your tips on WB and table parameter! I worked on the CFX tutorial - Oscillating Plate with Two-way Fluid Structure Interaction, and noticed the WB exports stepped pressure load in table parameter as you suggested. Following Edmund's suggestion, I ran a small case of concentrated load of table parameter on a cantilever beam to familiarize myself with the function. However, I encounterd an error message: "Present time 0 is less or equal to the previous time in a transient analysis." I am not sure what's really happening. Would you please comment on this? Thank you! Ryan And below is my APDL code: --------------------------------- /PREP7 *DIM,xforce,TABLE,8,1,1,TIME, !! !!time in sec !! xforce(1,0,1) =0 xforce(2,0,1) =1 xforce(3,0,1) =2 xforce(4,0,1) =2.0001 xforce(5,0,1) =3 xforce(6,0,1) =3.0001 xforce(7,0,1) =4 xforce(8,0,1) =5 !! !!force in x direction !! xforce(1,1,1) =0 xforce(2,1,1) =1 xforce(3,1,1) =1 xforce(4,1,1) =0 xforce(5,1,1) =0 xforce(6,1,1) =3 xforce(7,1,1) =3 xforce(8,1,1) =0 MP,EX,1,265e9 MP,PRXY,1,0.23 MP,DENS,1,3200 ET,1,SOLID45 BLOCK,0,100e-6,0,10e-6,0,2e-6 VMESH,ALL NSEL,S,LOC,X,0,1e-7 D,ALL,UX,0 D,ALL,UY,0 D,ALL,UZ,0 ALLSEL,ALL FINISH /SOLU ANTYPE,TRANS KBC,0 F,99,FZ,%xforce% SOLVE FINISH ---------------------------------

 January 23, 2012, 10:44 #7 Senior Member   Edmund Singer P.E. Join Date: Aug 2010 Location: Minneapolis, MN Posts: 512 Rep Power: 13 I am not seeing any time control in your scripting. Also, this error could be when you try a restart and you set the time to something other (smaller) that the restart file time. Either run this in a clean directory, or you can use the following command with ANTYPE to specify a new analysis. ANTYPE,TRANS,NEW To specify run time add: TIME,5 You will also need to specify the timestepping. Please look up the command NSUBST or DELTIM. Also readup on SOLCONTROL and AUTOTS. If you dont specify timestepping, ansys could autotimestep right over all of your BC changes. Be careful.

 February 2, 2012, 05:42 #8 New Member   Join Date: Jan 2011 Posts: 13 Rep Power: 8 Hi, Edmund and stumpy: Thank you for all your tips on my issue. I added 'AUTOS','DELTIM', and 'OUTRES' controls into my code, and the step loading can be reproduced correctly. I also tried the step loading in the FSI example of piezoelectric-actuated pump, and the analysis runs without problems. (http://www.kxcad.net/ansys/ANSYS/ans...COU_micro.html) Thanks again for your help! Ryan

 Thread Tools Display Modes Linear Mode

 Posting Rules You may not post new threads You may not post replies You may not post attachments You may not edit your posts BB code is On Smilies are On [IMG] code is On HTML code is OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post CKH OpenFOAM Running, Solving & CFD 12 March 21, 2016 14:05 jjc ANSYS 3 April 12, 2011 04:47 cyberbrain OpenFOAM 4 March 16, 2011 10:20 peiji1984 CFX 4 February 22, 2011 13:11 andyslee Main CFD Forum 0 January 29, 2003 00:39

All times are GMT -4. The time now is 06:05.