×
INTELLIGENT WORK FORUMS
FOR ENGINEERING PROFESSIONALS

Log In

Come Join Us!

Are you an
Engineering professional?
Join Eng-Tips Forums!
  • Talk With Other Members
  • Be Notified Of Responses
    To Your Posts
  • Keyword Search
  • One-Click Access To Your
    Favorite Forums
  • Automated Signatures
    On Your Posts
  • Best Of All, It's Free!
  • Students Click Here

*Eng-Tips's functionality depends on members receiving e-mail. By joining you are opting in to receive e-mail.

Posting Guidelines

Promoting, selling, recruiting, coursework and thesis posting is forbidden.

Students Click Here

Jobs

a question about field variable in vusdfld subroutine

a question about field variable in vusdfld subroutine

a question about field variable in vusdfld subroutine

(OP)
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.

RE: a question about field variable in vusdfld subroutine

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

RE: a question about field variable in vusdfld subroutine

(OP)
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

RE: a question about field variable in vusdfld subroutine

Hi,

Quote:

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

RE: a question about field variable in vusdfld subroutine

(OP)
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?

RE: a question about field variable in vusdfld subroutine

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

RE: a question about field variable in vusdfld subroutine

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

Red Flag This Post

Please let us know here why this post is inappropriate. Reasons such as off-topic, duplicates, flames, illegal, vulgar, or students posting their homework.

Red Flag Submitted

Thank you for helping keep Eng-Tips Forums free from inappropriate posts.
The Eng-Tips staff will check this out and take appropriate action.

Reply To This Thread

Posting in the Eng-Tips forums is a member-only feature.

Click Here to join Eng-Tips and talk with other members!


Resources