---

Hallo,

ich möchte die implizite Lösung in Abaqus gern mit der expliziten Lösung vergleichen und habe dafür einen einfachen Einmassenschwinger entworfen. Jetzt habe ich Probleme die statische Lösung, in der die Masse ausgelenkt wird, in die explizite Rechnung zu importieren.

Meine Input-Decks sehen folgendermaßen aus:

Statisch:

Code:

---

**
** --- BEGIN PART -----------------------------------------
**
*PART, NAME = PART_STATIC
**
*NODE, NSET = N_MASS
1, -0.5,  0.5,  0.5
2,  0.5,  0.5,  0.5
3,  0.5, -0.5,  0.5
4, -0.5, -0.5,  0.5
5, -0.5,  0.5, -0.5
6,  0.5,  0.5, -0.5
7,  0.5, -0.5, -0.5
8, -0.5, -0.5, -0.5
*NODE, NSET = N_NULL
10, -5.0,  0.0,  0.0
12,  5.0,  0.0,  0.0
*NODE, NSET = N_FREE
9, -0.5,  0.0,  0.0
11,  0.5,  0.0,  0.0
*ELEMENT, TYPE = C3D8, ELSET = E_MASS
1, 1, 2, 3, 4, 5, 6, 7, 8
*ELEMENT, TYPE = SPRINGA, ELSET = E_SPRING
2, 9, 10
*ELEMENT, TYPE = DASHPOTA, ELSET = E_DAMP
3, 11, 12
*SOLID SECTION, ELSET = E_MASS, MATERIAL = STEEL
*SPRING, ELSET = E_SPRING

1000000.0
*DASHPOT, ELSET = E_DAMP

1000.0
**
*END PART
**
** --- END PART -------------------------------------------
**
**
** --- BEGIN ASSEMBLY -------------------------------------
**
*ASSEMBLY, NAME = ASSEMBLY_STATIC
**
*INSTANCE, NAME = INSTANCE_PART_STATIC, PART = PART_STATIC
**
*EQUATION
5
9, 1, 1.0, 1, 1, -0.25, 4, 1, -0.25, 5, 1, -0.25,
8, 1, -0.25
5
11, 1, 1.0, 2, 1, -0.25, 3, 1, -0.25, 6, 1, -0.25,
7, 1, -0.25
**
*END INSTANCE
**
*END ASSEMBLY
**
** --- END ASSEMBLY ---------------------------------------
**
*MATERIAL, NAME = STEEL
*ELASTIC
2.1E11, 0.3
*DENSITY
7850.0
**
** --- Static Step ----------------------------------------
**
*RESTART, WRITE
*STEP, NLGEOM = YES, NAME = GENERAL_STATIC_STEP
*STATIC
*BOUNDARY
ASSEMBLY_STATIC.INSTANCE_PART_STATIC.N_NULL, 1, 3
ASSEMBLY_STATIC.INSTANCE_PART_STATIC.N_FREE, 2, 3
ASSEMBLY_STATIC.INSTANCE_PART_STATIC.N_MASS, 2, 3
ASSEMBLY_STATIC.INSTANCE_PART_STATIC.1, 1, 1, 0.5
*ENDSTEP
*

---

Diese läuft ohne Probleme, schicke ich dann jedoch die explizite Rechnung los bekomme ich Fehlermeldungen. Das Input-Deck:

Code:

---

*ASSEMBLY, NAME = ASSEMBLY_STATIC
**
*INSTANCE, INSTANCE = INSTANCE_PART_STATIC, LIBRARY = MASSE_STATIC
**
*IMPORT, STEP = 1, INCREMENT = 1, STATE = YES, UPDATE = NO
**
*END INSTANCE
**
*END ASSEMBLY
**
** --- Dynamic Step ---------------------------------------
**
*STEP, NAME = DYNAMIC_STEP, NLGEOM = YES
*DYNAMIC, EXPLICIT
, 10
*BOUNDARY, OP = NEW
ASSEMBLY_STATIC.INSTANCE_PART_STATIC.N_MASS, 2, 3
ASSEMBLY_STATIC.INSTANCE_PART_STATIC.N_NULL, 1, 3
ASSEMBLY_STATIC.INSTANCE_PART_STATIC.N_FREE, 2, 3
*DLOAD
ASSEMBLY_STATIC.INSTANCE_PART_STATIC.E_MASS, GRAV, 9.81, 0.0, 0.0, -1.0
*OUTPUT, FIELD
*NODEOUTPUT
U
*ENDSTEP
**

---

Ich bekomme folgende Meldungen:

Code:

---

***WARNING: THE OPTION *BOUNDARY,TYPE=DISPLACEMENT HAS BEEN USED; CHECK STATUS
            FILE BETWEEN STEPS FOR WARNINGS ON ANY JUMPS PRESCRIBED ACROSS THE
            STEPS IN DISPLACEMENT VALUES OF TRANSLATIONAL DOF. FOR ROTATIONAL
            DOF MAKE SURE THAT THERE ARE NO SUCH JUMPS. ALL JUMPS IN
            DISPLACEMENTS ACROSS STEPS ARE IGNORED

***ERROR: A BOUNDARY CONDITION HAS BEEN  SPECIFIED ON NODE SET
          ASSEMBLY_STATIC_INSTANCE_PART_STATIC_N_NULL BUT THIS NODE  SET IS
          NOT ACTIVE IN THE MODEL
***NOTE: DUE TO AN INPUT ERROR THE ANALYSIS PRE-PROCESSOR HAS BEEN UNABLE TO
          INTERPRET SOME DATA.  SUBSEQUENT ERRORS MAY BE CAUSED BY THIS OMISSION

***ERROR: A BOUNDARY CONDITION HAS BEEN  SPECIFIED ON NODE SET
          ASSEMBLY_STATIC_INSTANCE_PART_STATIC_N_FREE BUT THIS NODE  SET IS
          NOT ACTIVE IN THE MODEL
  *endstep

***ERROR: NODE SET ASSEMBLY_STATIC_INSTANCE_PART_STATIC_N_NULL HAS NOT BEEN
          DEFINED

***ERROR: NODE SET ASSEMBLY_STATIC_INSTANCE_PART_STATIC_N_NULL HAS NOT BEEN
          DEFINED

***ERROR: NODE SET ASSEMBLY_STATIC_INSTANCE_PART_STATIC_N_NULL HAS NOT BEEN
          DEFINED

***ERROR: NODE SET ASSEMBLY_STATIC_INSTANCE_PART_STATIC_N_FREE HAS NOT BEEN
          DEFINED

***ERROR: NODE SET ASSEMBLY_STATIC_INSTANCE_PART_STATIC_N_FREE HAS NOT BEEN
          DEFINED

---

Komischerweise gibt es keine Fehlermeldungen zum Knotenset N_MASS, das scheint zu funktionieren, woran könnte das liegen?

Eine Antwort auf diesen Beitrag verfassen (mit Zitat/Zitat des Beitrags) IP

---

Und was ist, wenn Du die Knotensets nochmal neu definierst ? Vielleicht werden Sets nicht im importiert.

------------------
Pam

Eine Antwort auf diesen Beitrag verfassen (mit Zitat/Zitat des Beitrags) IP

---

Also, ich habs mal folgendermaßen verändert:

Code:

---

**
*ASSEMBLY, NAME = ASSEMBLY_STATIC
**
*INSTANCE, INSTANCE = INSTANCE_PART_STATIC, LIBRARY = MASSE_STATIC
**
*IMPORT, STEP = 1, INCREMENT = 1, STATE = YES, UPDATE = YES
**
*END INSTANCE
**
*END ASSEMBLY
**
** --- Dynamic Step ---------------------------------------
**
*NSET, NSET = N_MASS
ASSEMBLY_STATIC.INSTANCE_PART_STATIC.1, ASSEMBLY_STATIC.INSTANCE_PART_STATIC.2, ASSEMBLY_STATIC.INSTANCE_PART_STATIC.3, ASSEMBLY_STATIC.INSTANCE_PART_STATIC.4, ASSEMBLY_STATIC.INSTANCE_PART_STATIC.5, ASSEMBLY_STATIC.INSTANCE_PART_STATIC.6, ASSEMBLY_STATIC.INSTANCE_PART_STATIC.7, ASSEMBLY_STATIC.INSTANCE_PART_STATIC.8
*NSET, NSET = N_NULL
ASSEMBLY_STATIC.INSTANCE_PART_STATIC.10, ASSEMBLY_STATIC.INSTANCE_PART_STATIC.12
*NSET, NSET = N_FREE
ASSEMBLY_STATIC.INSTANCE_PART_STATIC.9, ASSEMBLY_STATIC.INSTANCE_PART_STATIC.11
**
*STEP, NAME = DYNAMIC_STEP, NLGEOM = YES
*DYNAMIC, EXPLICIT
, 10
*BOUNDARY, OP = NEW
N_MASS, 2, 3
N_NULL, 1, 3
N_FREE, 2, 3
*DLOAD
ASSEMBLY_STATIC.INSTANCE_PART_STATIC.E_MASS, GRAV, 9.81, 0.0, 0.0, -1.0
*OUTPUT, FIELD
*NODEOUTPUT
U
*ENDSTEP
**

---

Bin mir nicht sicher ob es so richtig ist, arbeite zum ersten Mal mit Explicit.
Es kommen folgende Meldungen:

Code:

---

***WARNING: *TRANSFORM EXISTS AT SOME NODES IN THE ORIGINAL ANALYSIS. TO
            ENSURE CONTINUOUS DISPLACEMENTS AND VELOCITIES IDENTICAL
            TRANSFORMS MUST BE DEFINED AT THE NODES IN THE IMPORT ANALYSIS.
  *importnset
  *importelset
  *Heading
          Modell:  Masse                                                                                                                                                                                                                                                 
  *Nset, nset=ASSEMBLY_STATIC_N_FREE
  *Nset, nset=ASSEMBLY_STATIC_N_MASS
  *Nset, nset=ASSEMBLY_STATIC_N_NULL

***WARNING: IT IS RECOMMENDED THAT *SECTION CONTROLS, HOURGLASS=ENHANCED BE
            USED IN THE ORIGINAL ANALYSIS FOR CONSISTENT TREATMENT OF
            HOURGLASS FORCES IN BOTH ORIGINAL AS WELL AS IMPORT ANALYSES
  *output, field
  *Step, name=DYNAMIC_STEP, nlgeom=YES

***WARNING: NODE SET ASSEMBLY_STATIC_N_FREE HAS NO MEMBERS AND WILL BE
            IGNORED.  NODES DEFINED IN THIS SET MAY HAVE BEEN DELETED BECAUSE
            THEY WERE NOT CONNECTED TO ANY ELEMENTS.

***WARNING: NODE SET ASSEMBLY_STATIC_N_NULL HAS NO MEMBERS AND WILL BE
            IGNORED.  NODES DEFINED IN THIS SET MAY HAVE BEEN DELETED BECAUSE
            THEY WERE NOT CONNECTED TO ANY ELEMENTS.
  *Step, name=DYNAMIC_STEP, nlgeom=YES
  *dynamic, explicit
  *boundary, op=NEW
  *dload
  *output, field
  *nodeoutput
  *endstep
  *Step, name=DYNAMIC_STEP, nlgeom=YES
  *dynamic, explicit
  *boundary, op=NEW

***WARNING: THE OPTION *BOUNDARY,TYPE=DISPLACEMENT HAS BEEN USED; CHECK STATUS
            FILE BETWEEN STEPS FOR WARNINGS ON ANY JUMPS PRESCRIBED ACROSS THE
            STEPS IN DISPLACEMENT VALUES OF TRANSLATIONAL DOF. FOR ROTATIONAL
            DOF MAKE SURE THAT THERE ARE NO SUCH JUMPS. ALL JUMPS IN
            DISPLACEMENTS ACROSS STEPS ARE IGNORED

***ERROR: A BOUNDARY CONDITION HAS BEEN  SPECIFIED ON NODE SET
          ASSEMBLY_STATIC_N_NULL BUT THIS NODE  SET IS NOT ACTIVE IN THE MODEL
***NOTE: DUE TO AN INPUT ERROR THE ANALYSIS PRE-PROCESSOR HAS BEEN UNABLE TO
          INTERPRET SOME DATA.  SUBSEQUENT ERRORS MAY BE CAUSED BY THIS OMISSION

***ERROR: A BOUNDARY CONDITION HAS BEEN  SPECIFIED ON NODE SET
          ASSEMBLY_STATIC_N_FREE BUT THIS NODE  SET IS NOT ACTIVE IN THE MODEL
  *endstep

***ERROR: NODE SET ASSEMBLY_STATIC_N_NULL HAS NOT BEEN DEFINED

***ERROR: NODE SET ASSEMBLY_STATIC_N_NULL HAS NOT BEEN DEFINED

***ERROR: NODE SET ASSEMBLY_STATIC_N_NULL HAS NOT BEEN DEFINED

***ERROR: NODE SET ASSEMBLY_STATIC_N_FREE HAS NOT BEEN DEFINED

***ERROR: NODE SET ASSEMBLY_STATIC_N_FREE HAS NOT BEEN DEFINED

---

Es scheint irgendwie, als ob die Feder und der Dämpfer nicht in die Explicit-Analyse importiert werden.

Eine Antwort auf diesen Beitrag verfassen (mit Zitat/Zitat des Beitrags) IP

---

Ok, meine Vermutung war richtig, Abaqus/Explicit kann keine gewöhnlichen Feder- und Dämpferelemente nutzen, daher muss ich mit Connector-Elementen arbeiten.

Mein Input-File sieht folgendermaßen aus:

Code:

---

**
** --- BEGIN PART -----------------------------------------
**
*PART, NAME = PART_STATIC
**
*NODE, NSET = N_MASS
1, -0.5,  0.5,  0.5
2,  0.5,  0.5,  0.5
3,  0.5, -0.5,  0.5
4, -0.5, -0.5,  0.5
5, -0.5,  0.5, -0.5
6,  0.5,  0.5, -0.5
7,  0.5, -0.5, -0.5
8, -0.5, -0.5, -0.5
*NODE, NSET = N_NULL
10, -5.0,  0.0,  0.0
12,  5.0,  0.0,  0.0
*NODE, NSET = N_FREE
9, -0.5,  0.0,  0.0
11,  0.5,  0.0,  0.0
*ELEMENT, TYPE = C3D8, ELSET = E_MASS
1, 1, 2, 3, 4, 5, 6, 7, 8
*ELEMENT, TYPE = CONN3D2, ELSET = E_SPRING
2, 9, 10
*ELEMENT, TYPE = CONN3D2, ELSET = E_DAMP
3, 11, 12
*SOLID SECTION, ELSET = E_MASS, MATERIAL = STEEL
*CONNECTOR SECTION, ELSET = E_SPRING, BEHAVIOR = SPRING_BEHAVIOR
*CONNECTOR SECTION, ELSET = E_DAMP, BEHAVIOR = DAMP_BEHAVIOR
**
*END PART
**
** --- END PART -------------------------------------------
**
**
** --- BEGIN ASSEMBLY -------------------------------------
**
*ASSEMBLY, NAME = ASSEMBLY_STATIC
**
*INSTANCE, NAME = INSTANCE_PART_STATIC, PART = PART_STATIC
**
*EQUATION
5
9, 1, 1.0, 1, 1, -0.25, 4, 1, -0.25, 5, 1, -0.25,
8, 1, -0.25
5
11, 1, 1.0, 2, 1, -0.25, 3, 1, -0.25, 6, 1, -0.25,
7, 1, -0.25
**
*END INSTANCE
**
*END ASSEMBLY
**
** --- END ASSEMBLY ---------------------------------------
**
*CONNECTOR BEHAVIOR, NAME = SPRING_BEHAVIOR
*CONNECTOR ELASTICITY, COMPONENT = 1
1000000.0

**
*CONNECTOR BEHAVIOR, NAME = DAMP_BEHAVIOR
*CONNECTOR DAMPING, COMPONENT = 1, TYPE = STRUCTURAL
1000.0

**
*MATERIAL, NAME = STEEL
*ELASTIC
2.1E11, 0.3
*DENSITY
7850.0
**
** --- Static Step ----------------------------------------
**
*RESTART, WRITE
*STEP, NLGEOM = YES, NAME = GENERAL_STATIC_STEP
*STATIC
*BOUNDARY
ASSEMBLY_STATIC.INSTANCE_PART_STATIC.N_NULL, 1, 3
ASSEMBLY_STATIC.INSTANCE_PART_STATIC.N_FREE, 2, 3
ASSEMBLY_STATIC.INSTANCE_PART_STATIC.N_MASS, 2, 3
ASSEMBLY_STATIC.INSTANCE_PART_STATIC.1, 1, 1, 0.5
*OUTPUT, FIELD
*NODEOUTPUT, NSET = ASSEMBLY_STATIC.INSTANCE_PART_STATIC.N_MASS
U
*ENDSTEP
**

---

Allerdings bekomme ich folgende Fehlermeldung:

Code:

---

Error encountered when creating connector section definition for element set "ASSEMBLY_STATIC_INSTANCE_PART_STATIC_E_SPRING". OdbError: A connection type must be specified.

---

Die Connector-Karten haben nach dem Manual aber alle nötigen Parameter, Connector-Sections dürfen nur in den Bereichen Part, Instance und Assembly liegen, Connector-Behaviors nur im Model-Bereich, von daher weiss ich nicht wo mein Fehler liegen könnte.

Weiß irgendjemand Rat?

Eine Antwort auf diesen Beitrag verfassen (mit Zitat/Zitat des Beitrags) IP

---

Bei *Connector Section muss danach eine Datenzeile kommen, die den Connector-Typ definiert (z.B. Hinge, o.ä.).

In CAE gibt es im Interaction-Modul einen entsprechenden Button um diese Section zu erstellen. Auf diese wird beim erstellen des Connectors referenziert.

Eine Antwort auf diesen Beitrag verfassen (mit Zitat/Zitat des Beitrags) IP

---

Ok danke, das hat geholfen, ich habe jetzt als Basic translational type AXIAL gewählt, bin mir aber bei Basic Rotational connection component nicht sicher. Da mein erster Parameter translatorisch ist, muss der zweite rotatorisch sein. Ich habe verschiedene ausprobiert (UNIVERSAL, REVOLUTE, ROTATION) und bekomme immer wieder die Fehlermeldung:

Code:

---

Node X has zero rotary inertia but not all rotational degrees of freedom are constrained at this node. Please assign a physically reasonable rotary inertia to this node.

---

Die Meldung kommt bei allen 4 Knoten die für die Connector-Elemente benötigt werden, daher vermute ich, das bei dem 2. Parameter etwas nicht stimmt.

Eine Antwort auf diesen Beitrag verfassen (mit Zitat/Zitat des Beitrags) IP

---

Die Meldung ist doch eindeutig. Damit sich ein freier Knoten nicht beliebig drehen kann, braucht er etwas Trägheit oder eine Randbedingung.

Eine Antwort auf diesen Beitrag verfassen (mit Zitat/Zitat des Beitrags) IP

---

Hallo zusammen,

ich habe gestern vergeblich versucht, ein einfaches Feder-Dämpfer-Masse-System (siehe Anhang) aufzubauen und bin gnadenlos gescheitert.
Hat jemand vllt. ein einfaches Modell, das ich in Abaqus/CAE nachbauen kann bzw. meinem eigtl. gedachten Modell anpassen kann.

Vielen Dank im Voraus!!
(632)

Eine Antwort auf diesen Beitrag verfassen (mit Zitat/Zitat des Beitrags) IP