Radioss SPR Simulation: Unexpected Material Failure and Punch-Through Issues

Question

Hi everyone,

I am working on a Self-Piercing Riveting (SPR) process simulation using Altair Radioss (HyperMesh for pre-processing). I am experiencing an issue where the rivet (36MnB4) punches through the top sheet (Al5182) without proper penetration and interlock formation. Instead of the rivet flaring out and creating a mechanical bond, the top sheet undergoes premature failure (element deletion).

Model Details:

Materials: Both top and bottom sheets (2mm Al5182) and the rivet (36MnB4) are modeled using /MAT/LAW36 (PLAS_TAB) with experimental stress-strain data.

Properties: I am using P1_SHELL with Ishell=12 (QBAT) formulation to represent axial symmetric solid behavior.

Contact: INTERFACE TYPE 7 is used for all components with the following parameters:

Igap=2, Gapmin=0.05, Inacti=6

Istf=4, Stmin=1000, Idel=2

Failure Criteria: I have defined a failure model for the top sheet based on Max Plastic Strain (0.20) to simulate the piercing.

Boundary Conditions: Plunger and Blank Holder are controlled via IMPDISP with specific velocity curves (250 mm/s).

The Problem:During the simulation, as the rivet makes contact with the top sheet, the elements in the top sheet reach the failure strain too quickly, leading to a "clean cut" rather than the expected material flow and interlock. The rivet does not seem to deform or flare as it should according to the physical cross-section references.

Questions:

Is Max Plastic Strain (0.2) as a standalone failure criterion sufficient for SPR, or should I implement a more complex failure law like /FAIL/JOHNSON-COOK?

Does the Istf=4 (Stiffness scaling) in Type 7 contact potentially cause issues with high-strength rivets (36MnB4) penetrating softer aluminum (Al5182)?

Are there specific Ishell or Ithick settings I should verify to ensure the shell-to-solid (axial-symmetric) transition handles the high local compression better?

Any advice on stabilizing the material flow or adjusting the failure parameters would be greatly appreciated.

Thank you!

PierreChristophe_Altair · Answer

If you are using Quad elements and 2D analysis then:

* You must use /PROP/SOLID (or SOL_ORTH) and not /PROP/SHELL
* Compatible interfaces are type 1, 2, 3, and 5

See

https://help.altair.com/hwsolvers/rad/topics/solvers/rad/2d_3d_analysis_options_starter_r.htm

If you are planning to use SPH & Sol2SPH, then switch to 3D analysis and use SPH and/or BRICK elements instead of QUAD

Best regards

SuleOzgenc · Answer

spr hyper eng.pptx

Hi Pierre,

Thank you for your response. To clarify the model setup, I am using a 2D Axisymmetric formulation (N2D3D=1) and I have meshed the components with 2D Quad elements (not 3D solids).

Despite using a structured Quad mesh, the elements are still being deleted prematurely as the rivet penetrates the top sheet. This causes the "punch-through" effect instead of the expected material flow and interlock formation.

I have attached a PowerPoint presentation that contains detailed screenshots of my mesh density (0.15 mm), the material cards, and the current contact definitions (Type 7 and Type 11). I believe this will give you a better understanding of the instability I am facing.

Following your advice, I am now considering:

* SPH / SOL2SPH: To handle the extreme local strains at the rivet tip without element deletion.
* Failure Definition: Refining the /FAIL/BIQUAD parameters to allow for higher plastic strains before failure.

Could you please take a look at the attached slides and let me know if you see any specific conflict between my 2D Quad mesh and the interface settings?

Best regards,

Sule

PierreChristophe_Altair · Answer

Hi,

Would you clarify what you mean by "to represent axial symmetric solid behavior":

* Are you using 2D analysis type with Axisymmetric setting (N2D3D=1 in /ANALY)?
* Or are you trying to mimic axisymmetric conditions on a 3D analysis?

In first case, shell elements and interface type7 are not suited. In second case, I dont think shell elements be suited neither.

I would recommend instead SPH approach or solid approach with SOL2SPH activated (at least on the plate you try to pierce)

Regarding failure definition, be aware that Max Plastic Strain from /MAT/LAW36 is a global criterion that is independent from the strain/stress state of you material that is to say the plastic strain limit you define there is the same whether your material is in tension, compression or shear. I dont know the origin of the 20% limit you set, but it might be low for shear and compression modes. If you want to define a strain limit that depends on the stress state, you can indeed consider Johnson-Cook failure criterion or /FAIL/BIQUAD (which may be more accurate and simpler to adjust). See

https://community.altair.com/discussion/39220/fail-biquad-excel-to-visualize-the-failure-limit

And finally regarding your contact definition:

* Istf=4 is the appropriate setting
* Stmin=1000 should be OK if units are N/mm
* gap definition depends on the thickness of your plate and on the rivet modelling; yet 0.05 is quite small and attention should be paid to the time step and to how it is controlled

Best regards