Redefined material within a section 1

[9527]

Hi

Does anybody know how to reassign/redefine the material to a section during the next step.

This is what i am doing. Initial i have this layer of material "A" sitting on top of a substrate. Using the MODEL CHANGE, i would like to first remove that layer of material A and then redeposited a layer of material B. Hence i need to know how to change / redefine the material assign to that layer section in the following step.

thanks

Gabe

 

[mrgoldthorpe]

Set up two distinct sets of nodes and elements that occupy the same space. Name one element set 'ELSETA' and assign the material properties 'MATA'. Name the other element set 'ESETB' and give it the properties of 'MATB'

In the first step of your analysis REMOVE element set ELSETB, carry out the steps of your analysis using Material A properties. In the next step REMOVE element set ELSETA, followed by a step which a ADDs ELSETB. Now carry out your steps using Material B.
MRG

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

 

[9527]

Thanks MRG

Ummm so basically model/draw the two objects of different material occupying the same space initially then use the ADD and REMOVE to toggle between the two
sounds simple enough... i wondered whether that it will cause some sort of conflict or not (??!)

currently i am trying the *FIELD where initally i have defined two sets of material properties... so within keyword i will have

*Material A
*ELASTIC, DEPENDENCIES=1
50
*Conductivity, DEPENDENCIES=1
2
*Specific Heat, DEPENDENCIES=1
450
*Material B
*ELASTIC, DEPENDENCIES=2
90
*Conductivity, DEPENDENCIES=2
5
*Specific Heat, DEPENDENCIES=2
740

then i assign material A to it using
*INITIAL CONDITIONS, TYPE=FIELD, VARIABLE=1
Element

then within the STEP that i want to switch Element from material A to B I typed in
*FIELD, VARIABLE=2
ELEMENT

what do you think ? it this going to work ?

Gabriel

 

[mrgoldthorpe]

Gabe,
The FIELD option was originally going to be the second option to suggest to you; but not knowing the degree of non-linearity in your problem, I thought that it might lead to convergence difficulties. The element removal option replaces elements with equivalent nodal forces which it gradually relaxes during the step. This is a 'clean' way of simulating element removal.
On the other hand, switiching properties using FIELD variables could be rather abrupt and lead to problems in solution convergence.
Since you've started with the FIELD option you could at least try it out to see if it works. Let us know.
Regards,
MRG

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

 

[9527]

MRG

Umm i tried the FIELD option the way i have outlined it in my msg. It didn't work (not suprise). And i realized the following mistake that i have made "Dependencies # is not the same as Variable #" dependencies has nothing to do assigning variable number. So when i said *FIELD, Variable=2 i am not really changing it to material B.

From the manual, i think the variable numbers are assigned to the properties automatically (???) so in my case material A ELASTIC is 1, Conductivity is 2, Specific Heat is 3, and mat B Elastic is 4 and so on (not sure if this is indeed true) so i set the element intially to material A with *INITIAL CONDITION, TYPE=FIELD, Variable=1,2,3
then change it to mat B with *FIELD, Variable =4,5,6 .
And that's doesn't work either (i even try setting it with 3 different *Initial conditon and 3 *FIELD)

I wonder if *FIELD can do what i need (switch to a different material set) in the manual i see how they use FIELD to change the Elastic from one number to another within the same set (like changing the value that was like room temperature to a value that was say at 200)

I can't do what the manual is showing me because i am using temperature dependent material properties.
what do you think? Any suggestion?

I also have this problem, right now i am starting to try the over lay of 2 element to occupy the same space method. I have to use the TIE command to tie their interface together right (before i didn't have to becuse i model it with one big rectangle then i partition it to give me two distant cells) so yeah nothing has change expect i redraw the model with 2 rectangles , tie it looks good, heat transfer analysis good , but when i were to run the stress analysis (by reading in the nodal temperature from the heat analysis) i keep getting this error
File"Python/monitor Mechanism.py". line 392, in__processCB
File "Python/monitorMechanism.py", line 238, in shutdownandclose
File"<string>", line1, in recv

any idea what i am doing wrong ? how do i fix this ?

thanks
Gabe

 

[mrgoldthorpe]

Gabriel,
Regarding the FIELD issue, you have to use one field variable dependency as follows:

**
*ELASTIC, DEPENDENCIES=1
** set modulus for Material A when field variable is 1
** set modulus for Material B when field variable is 2
** E temp field_variable
50 , , 1.0
90 , , 2.0
**
*Conductivity, DEPENDENCIES=1
** set conductivity for Material A when field variable is 1
** set conductivity for Material B when field variable is 2
2 , , 1.0
5 , , 2.0
** etc.
*Specific Heat, DEPENDENCIES=1
450 , , 1.0
740 , , 2.0
** Of course, you can also include temperature dependency
** as well, but this example shows no variation with
** temperature.

** Use INITIAL CONDITIONS before your first step to set the
** field variables at all your nodes to 1:
*INITIAL CONDITIONS,TYPE=FIELD,VARIABLE=1
NALL, 1.0

** then in the step you wish to change from material A to B:
*FIELD, VARIABLE=1
NALL, 2.0
**
** from here on the field variable no. 1 is now 2 so the
** material B properties will be used.
** Beware of potential convergence difficulties!

Regarding the second method, I don't know what the error is.
However, you have to make sure nodal temperatures from the thermal analysis are available to the mechanical. So you must add and remove elements in the thermal analysis in exactly the same step sequence as the mechanical. See my previous answers to you last month in the thread:

http://www.eng-tips.com/viewthread.cfm?qid=102736

MRG

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

 

[9527]

MRG

I need to do it for temperature dependent material properties, so will it go something like this (NOTE that the second number / column is the temperature

*ELASTIC, DEPENDENCIES=2
50 , 10 , 1.0 (mat properties of A)
51 25 , 1.0
55 33 , 1.0
90 , -5 , 2.0 (of B)
88 10 , 2.0
66, 55 , 2.0

*Conductivity, DEPENDENCIES=2
2 , 20 , 1.0 (of A)
1 50 , 1.0
7 10 , 2.0 (of B)
5 , 15 , 2.0 (of B)
*Specific Heat, DEPENDENCIES=2
450 , 25 , 1.0 (of A)
480 27 , 1.0
520 30 , 1.0
740 , 20 , 2.0 (of B)
680 25 , 2.0

then i initially assign the ELEMENT SET to A by
*INITIAL CONDITION TYPE=FIELD, VARIABLE=1
ELEMENT, 1
(Question: i don't really get the VARIABLE=1 part.
since if have 3 different material properties, so do i
have three variables ? or is ALL material properties
consider as one variable? in other words in this
particular example do i need to say *Initial condition
type= field, variable=2 element, 1 to set the
conductivity then variable =3 to set specific heat? )

then when i need to switch the material B i type in
*FIELD Variable=1
ELEMENT, 2
(again do i need variable=2 and 3 to change
conductivity and specific heat)

hoping the PC will be smart enough to know that when i
say
*INITIAL CONDITION TYPE=FIELD VariABLE=1
ELEMENT, 1.0

it will use all material properties that has the
field variable equal to 1.0 (and pick one according to
temperature)

what do you think ?

Thanks for your help

Gabe

 

[mrgoldthorpe]

Gabriel,
Look at my last posting on 20/10/2004. You set the initial conditions and the values of the field variables at the nodes (though am not sure whether more recent versions of ABAQUS allow setting on element sets as you have indicated). 'NALL' is the element set of all nodes; though it could be just the nodes of the substrate.

It is DEPENDENCIES=1 since there is only 1 field variable to consider, that is VARIABLE 1. It is field variable number 1 switching from the value 1 to the value 2 that changes the properties of the material. You need no more field variables than no. 1.

By the way, in setting the material properties I can't remember whether you must first arrange properties in increasing order of temperature, then increasing field variable, or vice versa. Check the manual.

MRG

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

 

[mrgoldthorpe]

Correction to my last post. 'NALL' is the *node* set of all model nodes, or nodes in the substrate (not an element set).

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