Simplest way to restart a linear contact analysis in FEMAP/NX NASTRAN

[grandersen]

Hello,

I am working on a problem in FEMAP 2021.2/NX NASTRAN that involved various load conditions in a model that uses linear contacts. I wish to load a structure to obtain a displacement under one set of contacts. I then wish to apply a different load and change a couple of the contacts from a 'contact' to 'glued', and get a new displacement vector.

I'm not great with restarts, but I'm hoping it can be done this way. Can I restart into a 106 solution? Or do I have to go to a multistep solution?

I'm a bit lost. Any help would be appreciated.

 

[BlasMolero]

Dear Grandersen,
I understand you want to re-use the contact matrix in different types of analysis, correct?.
The solver Simcenter Nastran allows writing the contact matrix in DMIG format by including the parameter KGGCPCH = 1 in the BULK DATA SECTION (that is, PARAM, KGGCPCH, 1) of the Simcenter Nastran linear static analysis input file (SOL101). The solver writes the contact stiffness matrix from the last contact iteration in the PUNCH file in DMIG (Direct Matrix Input at Grids) format. This option is only available with the DIRECT SPARSE solver (the iterative solver does not support this option).

The DMIG matrix can be included in successive analysis by including the following line in the CASE CONTROL of the Simcenter Nastran input file: K2GG = KGGC

The benefits we obtain are the following:

• Include the contact effect in successive analyzes such as frequency analysis (SOL103) or forced response analysis (SOL111) without having to solve the contact problem again.
• Considerable savings in calculation time.

Best regards,
Blas.

~~~~~~~~~~~~~~~~~~~~~~
Blas Molero Hidalgo
Ingeniero Industrial
Director

IBERISA
48004 BILBAO (SPAIN)
WEB:

http://www.iberisa.com

Blog de FEMAP & NX Nastran:

http://iberisa.wordpress.com/

 

[grandersen]

Thanks much for the reply. I will try this.

I also need to use the deformations from the previous analysis as a starting point for the second analysis. Do you know if this can accommodated as well in a similar manner?

 

[BlasMolero]

Hello!,
For this you need to use the Multi-Step Structural Nonlinear Module (SOL401/402) that supports a combination of subcase types (linear, dynamic, preload, modal, Fourier, cyclic).
Multistep nonlinear solutions can have multiple subcases:
• These subcases can use the end state of the previous subcase as the initial condition for the next, this is called subcase chaining.
• For example, you may want to follow a bolt preload step with a contact step followed by a loads step with material nonlinearity

SUBCASE SEQUENCING
You can use the SEQDEP case control command to define any subcase type as sequentially dependent (SD), or non-sequentially dependent (NSD).
• With SOL401:An SD subcase can receive the final state variables from the previous static subcase. For example, plastic strains, creep strains, and displacements.
• With SOL402: An SD subcase uses the final computation state from the previous subcase for its starting state (for example, stress, strain, and displacements).

Solutions 401 and 402 add subcase chaining capability to Simcenter Nastran which will be familiar to users of other nonlinear solvers (for instance, abaqus). This differs from the standard behavior of linear solutions like SOL 101 where each subcase represents an independent simulation starting from the model’s initial zero state.

Best regards,
Blas.

~~~~~~~~~~~~~~~~~~~~~~
Blas Molero Hidalgo
Ingeniero Industrial
Director

IBERISA
48004 BILBAO (SPAIN)
WEB:

http://www.iberisa.com

Blog de FEMAP & NX Nastran:

http://iberisa.wordpress.com/

 

[grandersen]

OK, Blas, yes, I figured I would need 401 for this. Which we just got today! Thanks for you responses. I may soon have more questions.