a question about field variable in vusdfld subroutine 1

[zahedi66]

Hi there,
I come across with a problem,
I want to define friction coeff. tabular depend on field variable and filled the table. for example:
0.05 0.1
0.1 0.5
but I dont know how abaqus treat with field(nblock,nfield), is it consider field value in any element and assign a friction coeff. for that element?
thank you experts.

 

[akabarten]

Hi,

VUSDFLD subroutine defines field variable (FV) value for each integration point.
If you are using elements with reduce integration (only one integration point) then you have one FV value over element volume/area.
For fully integration elements you can have different FV values over element volume/area.

Contact is defined between point A and point B.
Point A is node on slave surface and point B is nearest point on master segment.
FV value for point A (FVa) is average value for all elements attached to the node.
FV value for point B (FVb) is interpolated for this point location base on values from the nearest integration points.
At the end FV value used to find friction coefficient will be average value (FVa+FVb)/2.

See abaqus documentation: Abaqus Analysis User's Manual, 36.1.5 Frictional behaviour, Using the default model

Regards,
Bartosz



VIM filetype plugin for Abaqus

https://github.com/gradzikb/vim-abaqus

 

[zahedi66]

thank you Bartosz,
I appreciate your profound understanding of the matter.
Let me to ask another question that I'm encountered:
If I want to depend two parameter (say Elasticity module and friction coefficient) on two different field variables say field(nblock,1) & field(nblock,2). how abaqus will treat? sequences should be considered in subroutine? shouldn't it?
regards

 

[akabarten]

Hi,

sequences should be considered in subroutine?

I have to say I do not understand completely your question.
Nevertheless please find some comments from my side.

Each FV value is treated by Abaqus in separate way in VUSDFLD subroutine.
You can set field(nblock,1) and next field(nblock,2) or the other way around.
The only important way is to set value for all used FV and for all material points (nblock).
Abaqus does not apply any default values, when you do not set field variable value numerical garbage can be set.

Regards,
Bartosz

VIM filetype plugin for Abaqus

https://github.com/gradzikb/vim-abaqus

 

[zahedi66]

as we know we don't specify a number for a field variable in CAE. so how abaqus recognize the order of field variables??
If I define a field variable for parameter A and then define another field variable for parameter B,
abaqus will assign field(nblock,1) values to A and field(nblock,2) to B?

 

[akabarten]

Hi,

In Abaqus is always only one 1st field variable (FV1), only one 2nd field variable (FV2), only one 3rd field variable (FV3) and so on.
FV1 is always field(nblock,1), FV2 is field(nblock,2), FV3 is field(nblock,3) and so on.
The same FV is used among all keywords which can be used with field dependencies.
It does not work in this way that FV1 under *ELASTIC is something different than FV1 under *FRICTION. Both FV1 are the same for Abaqus.
If you want to control elasticity with field variable and then control friction with different values you have to us FV1 for *ELASTIC and FV2 for *FRICTION.

I hope this is the answer for your question.

Regards,
Bartosz


VIM filetype plugin for Abaqus

https://github.com/gradzikb/vim-abaqus

 

[zahedi66]

Hi,
thank you Bartosz,
your answer really helped me,
I appreciate your free dispensing knowledge,
regards