availability of CONSTRAINED forces

[Michele]

Hello,

I have a model with a series of internal linear constrains, like the following:

---

*CONSTRAINED_LINEAR_GLOBAL
$#    licd
         1
$#     nid       dof      coef
      2982         2      -0.5
     18054         2      -0.5
      2983         2         1

---

The results of the simulation, in terms of displacements and stress results seems to be correct (compared with the solution performed on another software).

I need, as part of the solution, to postprocess the internal constraint forces. My question is: how can I know, taking the example shown above, the internal constraint force on node 2983 along dof 2 (and so on for other nodes/dof)?

Thanks

Michele

[James M. Kennedy]

Dear Michele,

 

See if this example is of some help:

 

https://www.dynaexamples.com/introduction/examples-manual/constrained/linear

 

Sincerely,

James M. Kennedy

KBS2 Inc.

February 17, 2021

--
You received this message because you are subscribed to the Google Groups "LS-DYNA2" group.
To unsubscribe from this group and stop receiving emails from it, send an email to ls-dyna2+u...@googlegroups.com.
To view this discussion on the web visit https://groups.google.com/d/msgid/ls-dyna2/576415ef-59b5-468f-81c9-ccb1bf6ccc31n%40googlegroups.com.

[James M. Kennedy]

Dear Michele,

 

*DATABASE_NODAL_FORCE_GROUP

Purpose: Define a nodal force group for output into the ASCII file nodfor. The output

interval must be specified using *DATABASE_NODFOR (see *DATABASE_OPTION).

 

Remarks:

1. The reaction forces in the global 𝑥, 𝑦, and 𝑧 directions (and local 𝑥, 𝑦, and 𝑧

directions if CID is defined above) for the nodal force group are written to the

nodfor file (see *DATABASE_NODFOR) along with the external work done by

these reaction forces. The reaction forces in the global 𝑥, 𝑦, and 𝑧 directions for

each node in the nodal force group are also written to nodfor. These forces can

be a result of applied boundary forces such as nodal point forces and pressure

boundary conditions, body forces, and contact interface forces. In the absence

of body forces, interior nodes would always yield a null force resultant vector.

In general this option would be used for surface nodes.

 

Sincerely,

James M. Kennedy

KBS2 Inc.

February 17, 2021

 

 

From: James M. Kennedy [mailto:j...@kbs2.com]
Sent: Wednesday, February 17, 2021 12:44 PM
To: 'Michele' <michele...@gmail.com>; 'LS-DYNA2' <ls-d...@googlegroups.com>
Subject: RE: [LS-DYNA2] availability of CONSTRAINED forces

 

Dear Michele,

 

See if this example is of some help:

 

https://www.dynaexamples.com/introduction/examples-manual/constrained/linear

 

Sincerely,

James M. Kennedy

KBS2 Inc.

February 17, 2021

 

From: ls-d...@googlegroups.com [mailto:ls-d...@googlegroups.com] On Behalf Of Michele
Sent: Wednesday, February 17, 2021 11:53 AM
To: LS-DYNA2 <ls-d...@googlegroups.com>
Subject: [LS-DYNA2] availability of CONSTRAINED forces

 

Hello,

--

[Michele]

Many thanks James,

   confirmed: the *DATABASE_NODFOR , once defined the nodes of interest (with *DATABASE_NODAL_FORCE_GROUP), is the solution for retrieving nodal external forces (in this case coming from the constraints).

There is a pending issue: the constraint can also impose a moment. How can I retrieve the nodal moments? (NODFOR just outputs x y z forces).

Yours sincerely

Michele

[James M. Kennedy]

Dear Michele,

 

A couple of suggestions:

 

https://www.dynasupport.com/howtos/general/force-analysis

 

Can you not make a cross section at locations where you want the moment info and use secforc database to get them?

 

-----------------------

 

A cross-section consists of a node set and one or more element sets. A node

set alone does not constitute a cross-section nor does an element set alone

constitute a cross-section.  

 

A correctly defined cross-section contains nodes which define the cutting

Surface and deformable elements to ONE SIDE of and touching that cutting

surface. Elements of rigid bodies do not contribute to cross-sections, that

is, only deformable elements should be included in cross-sections.

 

When the PLANE option is used to define a cross-section (*database_cross_

section_plane), LS-DYNA chooses the nodes and elements making up the cross-

section.   The nodes and elements chosen for that cross-section are reported

in the d3hsp file under the heading "interface definition".

 

*DATABASE_SECFORC determines the output interval for the cross-section forces

and moments. The forces and moments are output in the global coordinate system,

or, optionally, in an updated local coordinate system attached to a rigid body

or accelerometer.

 

As an alternative to defining a cross-section in the LS-DYNA input, in which

The cross-section follows a particular set of nodes and elements, you can use

the SPLANE option in LS-PREPOST  to gather forces/moments at  a cross-section

which is fixed in space. The sequence of LS-PREPOST operations is SPLANE >

(define location of cross-section) > CUT > FORCE > (select force or moment

component) > PLOT. When plotting forces via SPLANE in LS-PREPOST, the cutting

plane is fixed in space and does NOT  follow the deforming material. In other

words, the set of elements, which are cut can change  as the model deforms 

(the FixM option appears to have no effect). Also, force contributions come

only from those parts, which are displayed.

 

-----------------------

 

Sincerely,

James M. Kennedy

KBS2 Inc.

February 18, 2021

 

 

From: ls-d...@googlegroups.com [mailto:ls-d...@googlegroups.com] On Behalf Of Michele

Sent: Thursday, February 18, 2021 3:14 AM
To: LS-DYNA2 <ls-d...@googlegroups.com>

--

You received this message because you are subscribed to the Google Groups "LS-DYNA2" group.
To unsubscribe from this group and stop receiving emails from it, send an email to ls-dyna2+u...@googlegroups.com.

To view this discussion on the web visit https://groups.google.com/d/msgid/ls-dyna2/138f3743-35d1-48de-88ae-91e88b1de34an%40googlegroups.com.

[Michele]

Thank you James, good idea!

Best regards,

Michele

Il giorno giovedì 18 febbraio 2021 alle 18:49:09 UTC+1 jmk ha scritto:

Dear Michele,

 

A couple of suggestions: