Multi_step analysis not carrying over results from previous step 1

[sr1992]

Hi everyone,

I am trying to do a multi step analysis of a 1d beam.
In step-1, I add point load to the cantilever.
Step-2, thermal loading on the deformed cantilever, so as to induce buckling.

However, the results do not seem to follow this trend. The results from the 1st step dissipate as the Step-2 progresses. All the loads from step 1 are carrying over to step-2. In addition, in step-2, i have applied a fixed boundary constraint at the free end (force applied end in Step-1). Restart analysis is not an option for 1d beam elements in abaqus/standard.
I would be appreciative any help.
Thanks,

*Heading
** Job name: Job-237 Model name: Job-234
** Generated by: Abaqus/CAE 2019
*Preprint, echo=NO, model=NO, history=NO, contact=NO
**
** PARTS
**
*Part, name=Part-1
*Node
1, -1970., 0.
2, -1770., 0.
3, -1570., 0.
4, -1370., 0.
5, -1170., 0.
6, -970., 0.
7, -770., 0.
8, -570., 0.
9, -370., 0.
10, -170., 0.
11, 30., 0.
*Element, type=B21
1, 1, 2
2, 2, 3
3, 3, 4
4, 4, 5
5, 5, 6
6, 6, 7
7, 7, 8
8, 8, 9
9, 9, 10
10, 10, 11
*Nset, nset=Set-1, generate
1, 11, 1
*Elset, elset=Set-1, generate
1, 10, 1
*Nset, nset=Set-2, generate
1, 11, 1
*Elset, elset=Set-2, generate
1, 10, 1
** Section: Section-1 Profile: Profile-2
*Beam Section, elset=Set-1, material=Material-1, poisson = 0.3, temperature=GRADIENTS, section=CIRC
50.
0.,0.,-1.
*End Part
**
**
** ASSEMBLY
**
*Assembly, name=Assembly
**
*Instance, name=Part-1-1, part=Part-1
*End Instance
**
*Nset, nset=Set-1, instance=Part-1-1
1,
*Nset, nset=Set-2, instance=Part-1-1
11,
*End Assembly
**
** MATERIALS
**
*Material, name=Material-1
*Density
7.9e-09,
*Elastic
210000., 0.3
*Expansion
0.0005,
** ----------------------------------------------------------------
**
** STEP: Step-1
**
*Step, name=Step-1, nlgeom=YES
*Static
0.01, 1., 1e-05, 0.1
**
** BOUNDARY CONDITIONS
**
** Name: BC-1 Type: Symmetry/Antisymmetry/Encastre
*Boundary
Set-1, ENCASTRE
**
** LOADS
**
** Name: Load-1 Type: Concentrated force
*Cload
Set-2, 2, -15000.
**
** OUTPUT REQUESTS
**
*Restart, write, frequency=0
**
** FIELD OUTPUT: F-Output-1
**
*Output, field, variable=PRESELECT
**
** HISTORY OUTPUT: H-Output-1
**
*Output, history, variable=PRESELECT
*End Step
** ----------------------------------------------------------------
**
** STEP: Step-2
**
*Step, name=Step-2, nlgeom=YES
*Static
0.01, 1., 1e-05, 0.1
**
** BOUNDARY CONDITIONS
**
** Name: BC-2 Type: Displacement/Rotation
*Boundary
Set-2, 1, 1
Set-2, 2, 2
Set-2, 6, 6
**
** PREDEFINED FIELDS
**
** Name: Predefined Field-1 Type: Temperature
*Temperature
Part-1-1.Set-1, 500.
**
** OUTPUT REQUESTS
**
*Restart, write, frequency=0
**
** FIELD OUTPUT: F-Output-1
**
*Output, field
*Node Output
CF, NT, RF, U, UR, UT, V, VR
VT
*Element Output, directions=YES
LE, PE, PEEQ, PEMAG, S, TEMP
*Contact Output
CDISP, CSTRESS
**
** FIELD OUTPUT: F-Output-2
**
*Node Output
U, UR, UT, V, VR, VT
**
** HISTORY OUTPUT: H-Output-1
**
*Output, history, variable=PRESELECT
*End Step

 

[FEA way]

You can use Load Manager to deactivated the concentrated force in the second step.

 

[Mustaine3]

With the added BC in Step-2 you are forcing the node back to it's origin, since you enforce a position of zero, which is it's initial position.

If you want to fix it at the current position, you can use one of these two options:
- Apply a velocity BC with a value of zero
- Use a normal BC with the extra option "Fixed at current position" in A/CAE. With keywords it would be "*Boundary, Fixed".