Reactivating Element Set Using Model Change

[9527]

Hi

I am having this slight problem.
I am trying to use Abaqus to simulate the surface micromachining fabriaction process (where different layers of material are deposited at different temperature).

What I have is this, i have two "3D deformable solid" stacked on top of one another. Then initially/at the first step i remove the top layer using *model change, remove. Then i let the base subject to a heating load, where it under goes deformation / expansion. now in the next step i once again use *model change , add to reactiviate the top layer.

here is my problem, during the stress analysis, the layer of nodes shared by the base layer and the 2nd layer is displaced. The layer of nodes at the top of the 2nd layer is not displaced because they do not participate in the analysis steps in which the displacement is happening. Therefore, when the 2nd layer of elements is added back in, they do not conform to the profile one would like them to conform to.

according to the user manual this is suppose to happen because the 2nd layer's nodes were inactive during the displacement and this can be solve using boundary condition to "tie / constraint" the nodes together
but i don't know how to do it

anyone out there have any ideas for me?
thanks

Gabriel

 

[harry123456]

Hi
Maybe I dont understand your problem correctly, cant you tie the bases of the two layers using constraint---tie (in CAE) Then apply temperature to the base of the second layer and solve it in one step?
harry

 

[9527]

no no no ... that will not work.
because right now the two layers are tie no problem there
but since i would like to use *model change to mimic the deposition of new material, the top layer were initally deactivated making the nodes that are associated to that inactive. So even though there is a deformation in the base layer, when i reactivate the top layer at a layer step, it "no longer sits on top of the base layer" it is embedded and that's because the nodes were not active while the deformation took place.

thanks though
Gabriel

 

[mrgoldthorpe]

Gabriel,
A few questions:
- when you add the 2nd and any successive layers, are they supposed to be added in a strain-free condition and possibly at a different temperature to the subtrate?
- does the added layer have a uniform temperature?
- are you taking account of geometry change/large strain effects, via the NLGEOM option, or is it a small strain analysis?
- when you say the top layer is 'embedded', is that what you see when you view the mesh with magnified nodal displacements at the end of the step adding the 2nd layer?
Regards,
MRG

http://www.analysis.demon.co.uk

 

[mrgoldthorpe]

Gabriel,
If you read the ABAQUS manual you will see that for
*MODEL CHANGE,ADD=STRAIN FREE (the default) the strains and stresses in the added elements are based on the nodal deformations *after* the element addition, so the displacements of the bottom layer nodes before the addition of the 2nd layer are not relevant.

However, as you may have seen, when you view the mesh with magnified nodal displacements it may appear strange due, for example, to the thermal strains accumulated in the 1st layer before the addition of the 2nd layer. This is more a matter of presentation. However, the solution for the stress distribution throughout the model should be correct.

I have done analyses of multi-pass welding using the element removal and addition feature of ABAQUS. Due to the very large thermal strains involved it is not possible to obtain sensible plots of the deformed mesh.

Regards,
MRG

http://www.analysis.demon.co.uk

 

[9527]

MRG
thank you for much for taking the time to help me. ummm in regard to you first respone, i am going to explain my problem and hopefully you know what i am trying to do.

My goal is to look at the thermal residual stress due to fabrication process (basically stress due to change in temperature) of a multilayer micro mechanical electrical system. So i divde the task in 2 halves. One is the heat transfer analysis and then the stress analysis. First during the heat transfer analysis, i have one base and 2 layers. Initially i remove them all using *Model Change, then adding each layer back in at its desired step. I have the base initially at 25, heat it up to 240 using a concentrated heat source, then deposit layer 1 at 550 then layer 2 at 720. Then at a final step, i let it cool down to room temp by allowing free convection. The result looks good (what i would expect). So then i move to the static analysis.

Under Load, Field, i said use result from file and then i tell it the steps and increment to "match" it with the heat transfer analysis. Then i ran it. and then yeah, i see that during the heating of the substrate from 25 to 240, the substrate expanded so much that by the end of the step, the first layer is now embedded and after reading the manual, it said it is suppose to be like that because during the expanison, the layer 1 and 2 nodes are inactive therefore i won't move with the base layer.

so as for you questions:
1.yes it is strain free. Because i want to assume the new added layers are strain free initially and are interested in the strain that arise when you deposit a different material at a different temp on top of the substrate.
2. yes uniform temp
3. not sure what is needed. I mean my dimension are in micrometer so i figure the deflection are small, but i try trying turning on NLGEOM and i don't really see a different
4. when you say the top layer is 'embedded', is that what you see when you view the mesh with magnified nodal displacements at the end of the step adding the 2nd layer?
ummm when i view it, the scale factore was like 200, but if i view it as 1, i see no deflection at all

take a look at this (it is from example problem 1.1.10)
In problems involving geometric nonlinearities with
finite deformation, it is important to recognize that
element reactivation occurs in the configuration at
the start of the reactivation step. If the NLGEOM
parameter were used in this problem, the thickness of
the liner, when modeled with the continuum elements,
would have a value at reactivation that would be
different from its original value. This result would
happen because the outside nodes (the nodes on the
tunnel/liner interface) displace with the mesh,
whereas the inside nodes remain at their current
locations since liner elements are inactive initially.
This effect is not relevant in this problem because
geometric nonlinearities are not included. However, it
may be significant for problems involving finite
deformation, and it may lead to convergence problems
in cases where elements are severely distorted upon
reactivation. This problem would not occur in the
model with beam elements because they have only one
node through the thickness. In the model where the
liner is modeled with continuum elements, the problem
can be eliminated if the inner nodes are allowed to
follow the outer nodes prior to reactivation, which
can be accomplished by applying displacement boundary
conditions on the inner nodes. Alternatively, the
liner can be overlaid with (elastic) elements of very
low stiffness. These elements use the same nodes as
the liner but are so compliant that their effect on
the analysis is negligible when the liner is present.
They remain active throughout the analysis and ensure
that the inner nodes follow the outer nodes, thereby
preserving the liner thickness.

so yeah that's exactly what i am getting and i can't fix it using boundary conditions. But then after hearing what you said, that it (the deformation plot) doesn't really matter, the stress/strain should be correct right ???

Thanks for you help

Gabriel

 

[mrgoldthorpe]

Gabriel,

I see what you are doing. I'm a bit pushed for time today (going away tomorrow). However, I add a few points for you to consider to make sure your solution is correct.

1) You have to ensure that the nodes on layer 1 have an initial temperature of 550 degC so that when you add the layer 1 elements at 550 degC they are in a strain free condition. So I suggest that in both the thermal and mechanical analyses you have something like:
*INITIAL CONDITIONS, TYPE=TEMPERATURE
NLAY1 , 550.0
where the node set 'NLAY1' is all nodes on Layer 1.

2) Similarly, all the nodes in layer 2 need to set to an initial temperature of 720 in both thermal and mechanical analyses:
*INITIAL CONDITIONS, TYPE=TEMPERATURE
NLAY2 , 720.0
It is also useful to add a prior statement setting the initial temperature of the substrate nodes.

3) The problem is: the boundaries between the substrate and Layer 1, and between Layer 1 and Layer 2, have common nodes which will only take the last value you specify. You solve this by ensuring that you generate a mesh with unique, i.e. not shared, nodes at these two boundaries. The two sets of nodes at the Substrate/Layer 1 boundary have the same coordinates, however, as do the two sets of nodes at the Layer 1/Layer 2 boundary. So you use *EQUATION to tie them together as follows (and as suggested in your original post).

4) Lets say the (unsorted) set of nodes on the top of the Substrate is called 'NSUBTOP', the set of nodes at the bottom of Layer 1 is called 'NBOTLAY1', the set of nodes at the top of Layer 1 is 'NTOPLAY1', and finally the we have 'NBOTLAY2' at the bottom of layer 2.
In the thermal analysis you 'tie' the temperature degrees of freedom (dof 11) as follows:
*EQUATION
2
NBOTLAY1 , 11 , -1.0 , NSUBTOP , 11 , 1.0
2
NBOTLAY2 , 11 , -1.0 , NTOPLAY1 , 11 , 1.0

so when the relevant nodes are active the temperatures of the tied nodes are the same, but they have different initial temperatures.

In the mechanical analysis you 'tie' the displacement degrees of freedoms as follows:
*EQUATION
2
NBOTLAY1 , 1 , -1.0 , NSUBTOP , 1 , 1.0
2
NBOTLAY1 , 2 , -1.0 , NSUBTOP , 2 , 1.0
2
NBOTLAY1 , 3 , -1.0 , NSUBTOP , 3 , 1.0
(assuming it's a 3D model) and
*EQUATION
2
NBOTLAY2 , 1 , -1.0 , NTOPLAY1 , 1 , 1.0
2
NBOTLAY2 , 2 , -1.0 , NTOPLAY1 , 2 , 1.0
2
NBOTLAY2 , 3 , -1.0 , NTOPLAY1 , 3 , 1.0

5) You'll still get a strange magnified deformation plot because the displacements due to thermal strains are inconsistent in the 3 layers, but the resulting stresses should be satisfactory.

I hope this helps.
MRG

http://www.analysis.demon.co.uk

 

[9527]

MRG

Thanks you so much.... i am going to have to try it out (for i am unfamiliar with the EQUATION command)
thanks for all your help

Gabriel