Applying Initial Condition but non-cumulative results!

[amini06]

Dear member

Q : How could I have a cumulative result at the end of Transient –full Analysis?

Problem:

Let’s we have two loads acting on a cantilever beam, say F1: as a initial load & F2: as a new load.

If we apply F1 & F2 separately we have displacements D1 & D2, respectively. (for a node of the structure).
I use Transient-Full analysis, & use IC commands for establish initial condition caused by F1 (based on ANSYS-9.0 help files) used a small dummy time (=T1), two substeps & TIMINT.off and apply F2 as added load to system with a time T2. After each step the result was written in LSWRITE & finally used LSSOLVE to solve the loads cumulative.
Result is not cumulatively. I see a stepped result! Displacements from D1 at time zero changes to D2 at the end of T2 !
I expect D1 at zero time (as initial condition) & D1+D2 as a final result.

May you help me?

Thanks in advance
Amini

 

[meshparts]

Hello!

Did you thought about aplying F1+F2 in the second step?

Alex

 

[amini06]

Hi Alex
No.
Really I have a structure with a initial stresses caused by F1.this condition can be simulated by initial imposed displacement in the first step(D1).Then we apply new load,say F2.
So it is expected to have a diplacement equal to D1 + D2.Isn't it?

 

[meshparts]

I don't think so. Because initial conditions hold just at the beginning of the first step. For example, if you set 'timint,on', the structure will vibrate until it stops in the next steps. So I guess, the initial displacement becomes Null in the second step, without vibrations, since you set 'timint,off'.

 

[amini06]

Dear Mihaiupb
Thanks for ur attention.
We have two ways to apply imposed displacement.(D and IC commands).
With defining TIMINT,OFF (as it recommended ):
when I used IC command,the structure parameters changed from zero to F2's related parameters(i.e. from zero to D2)
when D command is used,the structure parameters changed from F1's related parameters to F2's ones(i.e. from D1 to D2)

How coulde I have a cumulative result?



About TIMINT,Off you can see the below comments(from 5.4. Performing a Full Transient Dynamic Analysis directory of ANSYS help Man.):

Nonzero initial displacement and zero initial velocity - This requires the use of two substeps (NSUBST,2) with a step change in imposed displacements (KBC,1). Without the step change (or with just one substep), the imposed displacements would vary directly with time, leading to a nonzero initial velocity. The example below shows how to apply uo = 1.0 and = 0.0:

...
TIMINT,OFF ! Time integration effects off for static solution
D,ALL,UY,1.0 ! Initial displacement = 1.0
TIME,.001 ! Small time interval
NSUBST,2 ! Two substeps
KBC,1 ! Stepped loads
LSWRITE ! Write load data to load step file (Jobname.S01)
! Transient solution
TIMINT,ON ! Time-integration effects on for transient solution
TIME,... ! Realistic time interval
DDELE,ALL,UY ! Remove displacement constraints
KBC,0 ! Ramped loads (if appropriate)
! Continue with normal transient solution procedures
...


Regards

 

[meshparts]

The simplest way is, like I said, to apply Forces, not displacements. You apply in the first step F1 and in the second one F1+F2 with ramped loads.

I think I understand what you want, but it ont work, since initial displacements are removed from the model in the second step. Even if you hold the initial displacement in the secon step, the force F2 will then have no influence, since forces and displacements on the same node are not compatible (either forces, or displacements).

 

[amini06]

Thanks Alex again:

That is right,if we want to apply the load,directly.But sometimes you are working with two programs(Ansys & another one).In this situations,sometimes(such as mine),the simplest way is to transfer displacements results from the first loading(by the first prog.)to ANSYS.
I don't know how we can do it,but maybe I should try with initial stresses files!?

Thanks in advanced,Alex.

 

[HStruct]

Hey Amini,

I had the same kind of situation, where I couldnt afford to apply forces but only the displacements as initial conditions.

I tried IC command but I didnt know it didnt hold displcements in next loadstep from the previous loadstep (I had more than 10 load steps)

Finally I am using initial stress file commands. Hopefully it will work for you if you have got the SUPPORTING KIND OF ELEMENTS IN YOUR MODEL because isfile and iswrite dont support allkinds of elements.

-HMT

 

[nodalDOF]

amini06 and Hstruct,


Did you guys try using the commands for applying cumulative loads?

for example

LS1
time,10
nsel,,,,1,10
F,all,FX,100 ! OR D,all,UX,1
solve

LS2
time,20
nsel,,,,1,10
FCUM,ADD ! Cumulative load now the load is 100-200
! OR DCUM
F,all,FX,100
solve





I think this will hold the model at previous state(end of LS1)

NodalDOF

 

[amini06]

Dear Nodaldof
Thanks.You are right.Your suggestion is useful for the same loads,as you mentioned above.But what is the solution if we deal with different loads?

Regards

 

[nodalDOF]

If you mean displacements in first LS and forces in second, Yes its not applicable. This was always a problem.