Can I define a constraint condition after deformation? 2

[bridgeclub]

In my problem, I have two part, I want to deform part1 then attach part1 to part2. In ABAQUS, I try to build up two steps, in step1 I try to apply a pressure to deform part1, then in step2 I want to define a constraint condition(tie) to attach part1 to part2.
The problem is: the constaint condition will be active from initial time and keep active through step1 and step2. So, I want to ask if someone know how to define a tie in certain time let it be active only in step2.

I appreciate if you reply and help.

 

[mrgoldthorpe]

bridgeclub,

I have never done this myself, but I think you can do this via surfaces. Define the two surface to be tied and the interaction. In the 1st step you de-activate the 'contact pair'. In the 2nd step re-activate it. Someone will correct me if I'm wrong.

So in the main input file you need:

** defne the two surfaces:
*SURFACE ...
*SURFACE ...
** define the contact pair and interaction, using the TIED
** option:
*CONTACT PAIR..
*SURFACE INTERACTION..

In the first step de-activate the interaction:

*MODEL CHANGE,REMOVE,TYPE=CONTACT PAIR...
**
** ..and in step 2 re-activate it:
*MODEL CHANGE,ADD,TYPE=CONTACT PAIR...

Consult the ABAQUS manual for details of the above commands.

Regards,

MRG

 

[corus]

An alternative, but longer method, would be to import the deformed part from the odb into a new model.

corus

 

[bridgeclub]

mrgoldthorpe:
Thank you for the reply.
I followed your suggestion to try to de-activate the tie condition in my problem, but try many commands all doesn't work. I tried *MODEL CHANGE,REMOVE,TYPE=TIE PAIR. and, follow this way tried many similar commands.
Do you know the right commands for tie condition?
Thanks.


corus:
Thank you for the reply.
I don't know how to try your way. How to input the deformed part from the odb into a new model? Could you give some detail suggestion?
Thanks.

 

[corus]

You need CAE in order to import a part from the odb

corus

 

[bridgeclub]

yes. I have ABAQUS CAE. How to operate or realize it? Could you tell more detail?

Thank you for help

 

[corus]

Try file/import/part

corus

 

[bridgeclub]

hi,corus
thank you for the help.
I can import a part from odb to a new model. but, problem comes, the part from odb loses its property and all stress, strain, and other deformed information. why it happen? do you have some ideas about this problem?

thanks for your time.

 

[mrgoldthorpe]

bridgeclub,

It looks like you are going along the importing the part route. However, here's an outline of the procedures required to do what you want using surface contact. You must refer to the on-line or paper manuals for detailed guidance on how you do this using CAE.

MRG

** In the model input part of the .inp file:
** Element set forming surface 1, the slave:
*ELSET,ELSET=ESURF1,GENERATE
1 , 100 , 1
** .. or whatever the element are comprising this surface
**
** Elements set forming surface 2, the master:
*ELSET,ELSET=ESURF2,GENERATE
101 , 200 , 1
** .. or whatever the element are comprising this surface
**
** Define the two surfaces:
*SURFACE , TYPE=ELEMENT , NAME=SURF1
ESURF1 ,
*SURFACE , TYPE=ELEMENT , NAME=SURF2
ESURF2 ,
** specifiy how they interact, and the name of the interaction:
*CONTACT PAIR, INTERACTION=INTTIED, ADJUST, TIED
SURF1 , SURF2
*SURFACE INTERACTION , NAME=INTTIED
**
**.. rest of model input
**
** Step 1
** remove the contact in step 1:
*MODEL CHANGE, REMOVE, TYPE=CONTACT PAIR
SURF1 , SURF2
** undertake the rest of the step...
**
** Step 2
** re-activate the contact in step 2:
*MODEL CHANGE, ADD, TYPE=CONTACT PAIR
SURF1 , SURF2
** and continue the step...
**

 

[bridgeclub]

mrgoldthorpe:
thank you.
it works.