On the Boundary Condition *Equation

[CSAPL]

I am applying Displacement BC throughc the contraints option
*Equations
However I need this to be applied only in a specific Step where in the following steps this Contraints should be eliminated.
Upon runing the analysis I got message :
"Error in job : in keyword *EQUATION, line 1402: The keyword is misplaced. It can be suboption for the following keyword(s): assembly, instance, part.
Please tell me what does that mean?
Have a happy 2007

 

[xerf]

As far as I know when you use constraints (e.g., *TIE, *EQUATION) they are enforced during entire analysis. They cannot be modified at the step level.

A specific keyword may be placed at specific level(s)(e.g. assembly level, step level etc.) of the .inp file. The documentation tells at what levels you you are allowed to place a specific keyword.

 

[CSAPL]

Thanks xerf. You are right... after careful looking at the Doc, *Equation must be introduced in the part or assembly edits , which means that it will be operated throughout the whole analysis. I am thinking of a solution to this issue.

 

[mrgoldthorpe]

CSAPL,
Would using TIED surfaces work as an alternative in your problem? In principle, you can add and remove ties in particular Steps. See the thread:

http://www.eng-tips.com/viewthread.cfm?qid=132367

Go to the end of the thread to see that the original poster got it to work.

 

[CSAPL]

Thanks mrgoldthorpe.
Just more Idea about my problem so that you may be able to help me overcome 2 weeks of disappointing solution attempts.
My problem seems similar to the one you have referred me to
(staged layers construction) so I built the whole model (in ONE PART ONLY)first and then removed all the layers except base which is subject to intitial stress.However during the first step ( which includes intial stress and Elements removal )i have found that the elements of the deactivated which are at the interface of the base have deformed. I beleive that i should use Surfaces and Tie Constraint

I will consult the manual on these issues and use them and let you know the outcome.

 

[CSAPL]

mrgoldthorpe thanks for your time and help
In your reply

http://www.eng-tips.com/viewthread.cfm?qid=132367

1-You seemed to define the Surf-1 (of part-1)consisting of several edges and Surf-2 (of part-2) consisting of different edges in CAE at Assembly level.as these two surfaces coincide(no gap)and both appear as one line. In such case How ( when defining surfaces in the assembly level) could one distinguish these two surfaces that appear as one line.
2-To overcome this issue I have defined a surface on the part level and follow your advice in that past thread:

*Tie, name=Constraint-1, adjust=yes
Part-2-1.S1BS, Part-1-1.FS
*End Assembly

*Step, name=Step-1
*Geostatic
*MODEL CHANGE, REMOVE, TYPE=CONTACT PAIR
Part-2-1.S1BS, Part-1-1.FS


However looking at the results, the Tie Constraint is still not deactivated.

 

[bfillery]

Dear CPSL

One thing I note from your last post is that you are applying a "tie constraint" rather than using a "tied contact pair formulation" that I believe the thread

http://www.eng-tips.com/viewthread.cfm?qid=132367

is refering to, and hence why the model change option to remove the "contact pair" is not working as hoped. This is only a guess, though you should check it out.

To form a "tied contact pair formulation", you need to create a contact pair, and following section 29.2.7 of the ABAQUS Analysis Users manual, for CAE usage:

"ABAQUS/CAE Usage: Interaction module: InteractionCreate: select a Slave Node/Surface Adjustment option: toggle on Tie adjusted surfaces"

Please read 29.2.7 of the ABAQUS Analysis Users manual for limitations etc.

bfillery

 

[mrgoldthorpe]

CSAPL,
bfillery makes a good point: the original thread showed how to set up a tied 'Contact Pair' and then remove and re-establish it.
In 1) of your last post, you refer to having 'no gap' between the two surfaces you wish to tie/untie. These are supposed to be separate surfaces, that is, they have different though possibly concident nodes. I'm not sure whether you resolved that in 2) or merely specified two surfaces sharing the same nodes.
Look at the diagrams below - I hope they format OK.

You require this:

| El1 | El2 |
.------.------.
.------.------. <--- these two horizontal planes are
| El3 | El4 | coincident. The 6 nodes (dots) are
distinct, though the 2 nodes in
each of the three pairs may be
coincident. There are two unique
surfaces that can be tied together.

Not this:

| El1 | El2 |
.------.------. <--- the elements on either side of
| El3 | El4 | the surface share the same nodes.
There is only one unique surface, so
a Contact Pair is not possible.

 

[CSAPL]

My humble understanding is that "tie constraint" implies rigid interface [full binding] between the two surfaces in which must be in full contact with each other.
Therfore "tie constraint" is a special cas of "tied contact pair formulation" in which the interface between the two surfaces (may have gab between them) may behave in elastic, elastoplastic ect manner
My problem is :
_____________________

Layer 1

----------------------
bottom elements course of Layer 1
_______________________
Layer 2


________________________



*Tie, name=Constraint-1, adjust=yes
Part-2-1.S1BS, Part-1-1.FS
*End Assembly

*Step, name=Step-1
** we have only layer 2 as Layer 1 is not built yet hence we deactivate Layer 1
*Geostatic
Model Change, Remove
Layer 1
** now remove the tie constraint to avoid the deforming of bottom elements course of layer 1 with the activated layer 2

*MODEL CHANGE, REMOVE, TYPE=CONTACT PAIR
Layer1 bottom-Surf, Layer2 top-Surf

*Step 2
* Static
** place layer 1 on the deformed Layer 2
Model Change,Add=Without strain
Layer 1
** re-activate the contact in step 2 to place Layer 1 on the top of the deformed layer 2 :
*MODEL CHANGE, ADD, TYPE=CONTACT PAIR
Layer1 bottom-Surf, Layer2 top-Surf

However the results show Layer 1 elements are deactivated
but bottom course is still deforming with the Layer 2.
Now the question does really Tie Constraint serve my purpose (texts of **)
This is what I mean by stage construction . Howvwer I am not sure if the above inp edits serve my purpose explained in the illustration of above edits (**
Any suggestion is highly appreciated

 

[mrgoldthorpe]

CSAPL,

The way you have described things above suggests that Layer1 and Layer2 share common nodes. In that case, *TIE or *CONTACT PAIR aren't applicable; they are used to tie together two *distinct* surfaces.

It sound like you want to put some pre-strain into a layer of elements, then add another layer, then add more load perhaps. If so, can't you do this build-up just using *MODEL CHANGE: adding elements in particular steps? I've done some multi-pass weld modelling in this way; though not using NLGEOM. Do you need to use NLGEOM?

I notice you have separate threads running on 'Model Change (Add/Remove Elements)' and 'On dividing a part into different parts'. I wonder if it would be helpful if you explained what you want to accomplish with your model.

 

[CSAPL]

Thanks mrgoldthorpe
I am glad that finally someone got me
I am doing staged construction ( height increases with time) of an embankment. Layer 2 is the foundation on which the embankment of differnt layers to be built (Layer 1 , layer 3 ..and so on). Yes I need NLGEOM becuase the materials are very soft (large strain is expected).
if we donnot need *TIE or *CONTACT PAIR. How do we solve the strain occuring in layer one (deactivated one) in the Step 1. Particulrly knowing the Layer 2 will experience high deformation.
In the Step 2 I do not think (I am not sure)that I Should add Layer 1 with Strain as this layer will feel strain only placing it on the layer 2 (since the moment it is activated ,begining of Step 2) rather than the moment the
the analysis starts (begining of Step 1)
Layer 1 should be deactivated in a manner fitting the deformed layer undeneath (layer 2)
Please advice . I highly appreciate your generous help and support

 

[CSAPL]

The Model with NLGEOM never converges in spite of hugly relaxing the convergence criterion and applying artifical damping to the model to supress the instability.
How to solve this convergence problem

 

[mrgoldthorpe]

CSAPL,

A few questions/points to consider:

Is NLGEOM necessary? What output parameters do you require from the model and how do you think they are affected by modelling non-linear geometrical behaviour rather than small strain/displacement? Do you have sufficiently accurate material data at large strains? Are the large strains important, or is the non-linear geometry behaviour most important?

At which point do you start to see poor convergence? Is it solving for the first layer, 2nd layer or 3rd etc?

In this particular analysis you say is giving problems, are you using constraints or simply adding in new layers of material by adding elements?

Have you read section 7.5.1, Element and contact pair removal and reactivation" (in Manual of Version 6.5):

Large-displacement analysis
In large-displacement analysis the new configuration can be significantly different from the original configuration specified in the model definition. The change in configuration may result from large deformation or rigid body motion. For the nodes of the reactivated elements to be in the correct position upon reactivation, these nodes must be shared by elements that are not removed. Otherwise, the nodes of the removed elements remain at the location occupied at the time of removal. For cases where an enclosed region of material is reactivated, the shared-node restriction may require that a duplicate set of elements whose material properties do not influence the stress solution be defined on top of the removed elements. These duplicate elements provide a means of tracking the position of the nodes of the removed elements.

Sorry about not providing an answer, but I don't know all the details of your problem. If I was you, I'd be tempted to sort out issues and obtains initial solutions without NLGEOM.