restart option 2

[jiligeo]

Hi there,
I am doing a nonlinear analys and I am interesting to apply loads in different steps. I mean at the fist step self weight of structure and at the second step live loads. Do you know any example which use restart option?

Thanks
Jili

 

[Drej]

Even easier is to use:

/solu
time,1
! antype,static (for example)
! apply self weight load (acel,...)
! set boundary conditions
! outres etc.
solve

time,2
! apply live loads
! set boundary conditions
! outres etc.
solve

save
fini


------------
See faq569-1083 for details on how to make best use of Eng-Tips.com

 

[jiligeo]

Thank you very much for your applicable answers.
I have analysed the model using the time command.
The new problem which I have is:

How can I set the deformations to zero before starting a new load step?

In plaxis program it is possible with an option (Reset displacement to zero) in every load step. Is it possible in ANSYS too?
I have to reset the deformations causing the self weight to zero because in reality the dimensions of structure that we have are considering (after) the effect of self weight and in soil mechanics this deformations are high.

Regards
Jili

 

[roypersa]

I really don't understand your problem but if you want to set displacements to zero try:
IC,ALL,ALL,0

Best Regards,

roypersa

 

[jiligeo]

Dear roypersa,
thank you for your answer.
I am modelling the effect of a tunnel construction on a building. I have two load steps and I need the difference deformation between them.

In the first load step I define the self weight of soil and structure and it cause about 10 cm deformation. Actually, these deformations had done 50 years before and have not any effect because the dimensions of model are after these deformations but the stresses are important because I use the DP material model and the soil material has internal friction.

In the second load step: I define the tunnel construction using element dead. Displacements in this step are important for me and it is less than 2 cm.
If I do not set the deformations after first step to zero the results are not true (more than 10 cm) because most of them are from fist load step.

Actually I need the difference deformation between two load steps.
In plaxis program it is possible with an option (Reset displacement to zero) for every load step.
I hope to explain my problem well.

Regards
Jili

 

[roypersa]

Jili,

If I understood correctly, you are trying to run several static analyses, thus the command line I sent you before will do.
Referring to the example that Drej sent before:
.
.
.
time,2
! apply live loads
! set boundary conditions
! unselect nodes with constrained DOF (suggestion since DOF constraint should override the IC command)
ic,all,all,0
! reselect everything
! outres etc.
solve

Hope it helps. Best Regards,

roypersa

 

[Drej]

jiligeo/roypersa,

Please note that the IC command will not work since it is not valid in the second load step of an analysis (the "initial conditions" description gives it away I suppose).

The command you need to zero the displacements is UPCOORD. Please see the help file for a description.


------------
See faq569-1083 for details on how to make best use of Eng-Tips.com

 

[roypersa]

Drej,
I always wondered about the name of that command . You are right, it won't work from the second load step.

Jili,
I am still confused about your problem, looks like you don't want to include the effects of the first load case in your second one. If that is your goal, you should only need to reset the loads (lsclear,all) not the displacements. However you have stated that your results are actually adding up, are you specifying the analysis to be transient? (antype,4).

roypersa

 

[jiligeo]

Dear roypersa,
thanks a lot for your time,
As you know in Drucker-Prager material model the strength of material depends to the stresses (because of internal friction of soil). Therefore I have to do the first load step. But only the deformation in second load step is important for me and I need the difference deformations between load step 2 and 1. In the other words the first load step applied to the model at least for 50 years and the dimensions of model that I have are after these deformations but the effect of stresses are still in structure.

Regards
Jili