2D Axisymmetric – Line-to-Line Contact in HyperMesh v2024?

simonsgl · 2025-05-12T12:19:11+00:00

There was an error rendering this rich post.

Hello everyone,

I’m currently working on a 2D axisymmetric simulation in Altair HyperMesh where I want to model the nonlinear penetration of a hard cutting edge into a softer elastomeric sealing material. The goal is to capture the realistic contact behavior during the initial intrusion and deformation phase.

I came across a tutorial from version 2021 where the contact between two lines was defined using a line-to-line contact approach. However, that tutorial was based on the older user interface. (OS-T: 1394 Axi-Symmetric Ball Joint)

Now I’m working in Altair HyperMesh v2024 and I’m having trouble locating the corresponding feature.
Where exactly can I define line-to-line contact in the new interface in v2024?
Is there any updated workflow or specific card I need to use in the current HyperWorks environment?

I’ve attached an image of the geometry I’m trying to simulate for better understanding.

Any help or pointers to updated documentation would be greatly appreciated!

Best regards

Simon

Find more posts tagged with

HyperMesh

v2024

Accepted answers

All comments

solon

Hello,

You can create a contact where the two SURFS will reference FE edges.

You can follow the following verification problem for reference:

https://help.altair.com/hwsolvers/os/topics/solvers/os/nafems_nonlinear_static_analysis_axisymmetric_elements_interference_2_cylinders_r.htm?zoom_highlight=Axisymmetric

simonsgl

Thanks for your response!

I do see an option called "By Edge" when creating a contact surface, but it seems to select the entire elements adjacent to the edge, rather than referencing the edge line itself.
As a result, the contact is applied to the element surface, not directly to the FE edge, which doesn’t seem to behave like a true line-to-line contact (as shown in the screenshot I shared).

Is there a different way to define a surface that references only the FE edges?

Thanks again for the support!

solon

Have a look at the attached recording.

Recording 2025-05-12 171535.mp4

simonsgl

I found the correct way to define the FE edge-based contact surfaces – thank you for pointing me in the right direction!

However, my simulation still isn't working as expected. The cutting edge does not seem to displace or deform the seal properly, as if the contact isn't being enforced correctly.

I created one master and one slave surface for both the top and bottom contact regions, but the interaction doesn't look physical – the bodies just overlap without significant resistance or deformation.

I've attached both my .hm and .h3d files in case someone might spot an obvious mistake in my setup.
Any insights would be greatly appreciated!

Thanks again for the support.

CF_Flansch.hm

CF_FlanschV1.h3d

solon

Axisymmetric analysis requires the bellow elements-properties:

You can follow the following verification problem for reference:

https://community.altair.com/home/leaving?allowTrusted=1&target=https%3A%2F%2Fhelp.altair.com%2Fhwsolvers%2Fos%2Ftopics%2Fsolvers%2Fos%2Fnafems_nonlinear_static_analysis_axisymmetric_elements_interference_2_cylinders_r.htm%3Fzoom_highlight%3DAxisymmetric

simonsgl

Thanks for your reply!

You're absolutely right about the requirements for axisymmetric analysis.
However, just to clarify – wouldn't it also be possible to first run the simulation in a simplified 2D planar setup, purely for testing purposes?

I understand that this wouldn't produce a proper 3D axisymmetric visualization in the results, but shouldn't the actual penetration behavior still be represented correctly, at least in terms of contact interaction and deformation?

I'm mainly trying to verify whether the contact is working as expected before moving on to the full axisymmetric setup.

Thanks again for your input!

solon

The option works for contact in plane stress, plane strain, and axisymmetric 2D analysis.

simonsgl

Hi everyone,

I've implemented the contact definition as discussed in earlier threads, using FE edge-based contact surfaces for my axisymmetric setup.

However, since I initially built the model in the wrong plane (not X–Y), I had to rotate the geometry by 90 degrees to align it properly for axisymmetric analysis using QAXI elements.

Now, when I run the simulation, I get the following error:

*** ERROR # 6531 ***
The main of CONTACT 1 is defined on element(s) with incorrect
node numbering (e.g., element 8).

I've tried reviewing the affected elements and contact surfaces, but I haven’t been able to resolve the issue.
I’ve attached my .hm file to this post in case someone is able to take a look.

Any suggestions on how to fix this node numbering issue or properly orient the elements for axisymmetric contact would be greatly appreciated!

Thanks in advance for your help.

CF_Flansch_14.05.25.hm

solon

Hello,

The two surfaces should have the same normal.

Reverse the normal of the component 1 elements and redefine the SURFs of contact edges.

This should fix the incorrect node numbering.

simonsgl

Thanks for the fast answer!

ich reversed the normals of the component but the error is still there.

Is there any other method to solve the problem? I tried also to renumber the nodes with "renumbering".

solon

Hi,

After reversing the normal, the FE edges in the SURF sets are changed. You have to reselect the correct FE edges.

simonsgl

I deleted the SURF sets and the contacts completely and reselectet it.

The error is still the same.

"The secondary of CONTACT 1 is defined on element(s) with incorrect
node numbering (e.g., element 23227)."

I'm currently stuck and unsure what further steps I can take to make the simulation work.

CF_Flansch_14.05.25.hm

solon

I am using Optistruct version 2025. You can find the model with the changes mentioned attached:

CF_Flansch_14.05.25.fem

simonsgl

First of all, thank you very much for helping me identify and solve the issue with the contact setup in my axisymmetric model – I really appreciate the support!

However, I’m still a bit unsure about something:
I was able to get a working version of the model using the .fem file, but I’m wondering if it makes a difference for me to continue working with your .fem file instead of the .hm file, especially considering that I still need to:

assign different materials
possibly modify the mesh in some areas

Also, I must admit I still haven’t fully understood how to resolve the original contact problem in my own model. It seems like such a simple fix, but I can’t reproduce the working setup properly yet.

Thanks again in advance!

solon

The elements' normal should point to the positive z-axis when you model in X-Y plane.

There is a relevant Warning message in the .out file:

simonsgl

I tried to reverse the normals of the upper flange, but unfortunately I can't – they seem to be linked to the geometry, so the option is grayed out or doesn’t apply.

Is there a way to detach the elements from the geometry so I can reverse the normals independently?

If not, I’ll just continue working with the .fem file you provided, since I think I can make all necessary adjustments there as well (e.g., materials, mesh changes).

Thanks again for your help!

solon

You can reverse the normal of the surface:

simonsgl

Hi everyone,

I finally managed to get my axisymmetric contact simulation to work properly. With a linear elastic material model, the results look reasonable and stable – the contact behavior appears correct.

However, when I switch to a nonlinear material model (for the softer sealing element), the elements start to distort excessively, and the results become unrealistic – see the attached image for reference.

Could this be due to the element size (too coarse for large deformation)? Or is there something else I should adjust in the simulation settings to improve the robustness when using nonlinear material properties?

I’ve attached the .hm file, the .out file, and the .h3d result file for reference.

Hello,

You can activate Finite Sliding (TRACK= CONSLI) option for the contacts. For TRACK=CONSLI, termed continuous sliding, the contact search is done for every iteration. The CONSLI option is expected to produce more accurate results and, in some cases, better convergence robustness, especially when very large sliding and/or distortion is present.

simonsgl

Hi everyone,

So far my axisymmetric contact simulation was running well and gave reasonable results. However, after modifying the material properties, I’ve started to experience convergence issues.

One material is now very stiff, and the other one is very soft . Since this change, the solver struggles with convergence – especially during the contact phase.

I’ve already tried adjusting the contact parameters, for example by setting PCONT to SOFT, but the issue persists.

Since the same setup worked fine before the material change, I assume the problem is related to the large stiffness ratio between the two materials.

My qestions:

Are there recommended techniques in OptiStruct to handle high stiffness contrasts in contact problems?
Would mesh refinement in the soft body help?
Is there a way to stabilize the solution without overly softening the contact?

Any advice would

be appreciated!

Thanks in advance

CF_Flansch_02.07.hm