CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > CFX

MFX FSI: How to apply time-varying load?

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

Reply
 
LinkBack Thread Tools Display Modes
Old   December 16, 2011, 13:18
Default MFX FSI: How to apply time-varying load?
  #1
New Member
 
Join Date: Jan 2011
Posts: 13
Rep Power: 6
gogohusky is on a distinguished road
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
gogohusky is offline   Reply With Quote

Old   December 20, 2011, 11:59
Default
  #2
Senior Member
 
Join Date: Apr 2009
Posts: 516
Rep Power: 12
stumpy is on a distinguished road
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.
stumpy is offline   Reply With Quote

Old   January 18, 2012, 11:01
Default
  #3
New Member
 
Join Date: Jan 2011
Posts: 13
Rep Power: 6
gogohusky is on a distinguished road
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
gogohusky is offline   Reply With Quote

Old   January 18, 2012, 15:01
Default
  #4
Senior Member
 
Join Date: Apr 2009
Posts: 516
Rep Power: 12
stumpy is on a distinguished road
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.
stumpy is offline   Reply With Quote

Old   January 19, 2012, 14:48
Default
  #5
Senior Member
 
Edmund Singer P.E.
Join Date: Aug 2010
Location: Minneapolis, MN
Posts: 495
Rep Power: 11
singer1812 is on a distinguished road
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%
singer1812 is offline   Reply With Quote

Old   January 23, 2012, 10:29
Default
  #6
New Member
 
Join Date: Jan 2011
Posts: 13
Rep Power: 6
gogohusky is on a distinguished road
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
---------------------------------
gogohusky is offline   Reply With Quote

Old   January 23, 2012, 10:44
Default
  #7
Senior Member
 
Edmund Singer P.E.
Join Date: Aug 2010
Location: Minneapolis, MN
Posts: 495
Rep Power: 11
singer1812 is on a distinguished road
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.
singer1812 is offline   Reply With Quote

Old   February 2, 2012, 05:42
Default
  #8
New Member
 
Join Date: Jan 2011
Posts: 13
Rep Power: 6
gogohusky is on a distinguished road
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
gogohusky is offline   Reply With Quote

Reply

Thread Tools
Display Modes

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 Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Multiple floating objects CKH OpenFOAM 10 September 21, 2011 23:13
How to model concrete slab in ANSYS and apply 2 million cyclic load. jjc ANSYS 3 April 12, 2011 04:47
Full pipe 3D using icoFoam cyberbrain OpenFOAM 4 March 16, 2011 10:20
MFX FSI for linear case. Help needed. peiji1984 CFX 4 February 22, 2011 13:11
Is it possible apply AC and DC at the same time andyslee Main CFD Forum 0 January 29, 2003 00:39


All times are GMT -4. The time now is 23:56.