🎉Community Raffle - Win $25

An exclusive raffle opportunity for active members like you! Complete your profile, answer questions and get your first accepted badge to enter the raffle.

Join and Win

Question about Contact and Compression Support Only

Rod

Hi there.

I hope someone will help me finish my model.

I am analyzing a beam that will move the entire wind tunnel support jacket. See first picture.

This beam is placed on top of the SPMT truck. See second picture.

My question is:

A. How to I model the contact between the top of the long beam and bottom of the bracket (second picture denoted as A). I am getting an error 'Undefined SET SSID on CONTACT 1' but I already defined it. I don't know what am I missing.

B. The boundary condition will be placed at the wood locations. This will be in compression only condition. How do I model that?

I am attaching my model (only half have been modeled yet).

image.png.967156429ac4d1583248417166f39421.png

<?xml version="1.0" encoding="UTF-8"?>

Unable to find an attachment - read this blog

Find more posts tagged with

English

HyperMesh

Accepted answers

All comments

Rod

Update:

I was able to solve the contact part. The only thing I need to solve is how to model the support condition (compression only).

Thanks

Simon Križnik

Hi,

the 'Undefined SET SSID on CONTACT' error was due to contact surfaces having inappropriate card image- SURF should be used instead of ELIST.

The compression-only boundary condition can be created by duplicating, offsetting and constraining a set of elements in the region where contact is expected to model the upper support surface of the SPMT truck. Define a contact interface between support and the bottom plate. Contacts should also have friction to prevent slipping, which could result in rigid body motion.

Sliding contact might not work using linear static analysis. In linear static analysis, the contact status does not change, does not slide and the contact stiffness is constant. Therefore, a nonlinear quasistatic analysis (NLSTAT) should be used. If no liftoff is expected then linear static analysis can be used.

There were some other modeling issues:
-the symmetry boundary conditions were inappropriate. To constrain in the YZ plane, only X translation and Y & Z rotations should be constrained.
-'dummy' material has no density
-single point constraints and forces were in the same load collector '400 ton Weight', but they should be separated. Also, forces were applied to the same nodes as constraints, which cancels the effect of forces.
-the pyramids of contact surfaces should be pointing in the direction of contact with MORIENT=NORM

Unable to find an attachment - read this blog

Rod

Wow, thanks a lot man! You went as far as correcting my model. Your reply is extremely helpful.

Rod

Hi,

the 'Undefined SET SSID on CONTACT' error was due to contact surfaces having inappropriate card image- SURF should be used instead of ELIST.

The compression-only boundary condition can be created by duplicating, offsetting and constraining a set of elements in the region where contact is expected to model the upper support surface of the SPMT truck. Define a contact interface between support and the bottom plate. Contacts should also have friction to prevent slipping, which could result in rigid body motion.

Sliding contact might not work using linear static analysis. In linear static analysis, the contact status does not change, does not slide and the contact stiffness is constant. Therefore, a nonlinear quasistatic analysis (NLSTAT) should be used. If no liftoff is expected then linear static analysis can be used.

There were some other modeling issues:
-the symmetry boundary conditions were inappropriate. To constrain in the YZ plane, only X translation and Y & Z rotations should be constrained.
-'dummy' material has no density
-single point constraints and forces were in the same load collector '400 ton Weight', but they should be separated. Also, forces were applied to the same nodes as constraints, which cancels the effect of forces.
-the pyramids of contact surfaces should be pointing in the direction of contact with MORIENT=NORM

Unable to find an attachment - read this blog

Rod

Hi there.

I updated my model with all your suggestions. The problem I am having now is that the solutions don't converge.

Probably because of lack of supports? Are there ways to solve this one?

I am attaching my final model.

Thanks in advance.

Unable to find an attachment - read this blog

Simon Križnik

Glad to help.

Yes, usually models experience convergence difficulties if they are not properly constrained. This is especially problematic with models constrained only by contact.

The following changes were made to make the model converge:
-the main issue was that the girder was split at the midpoint. Shift+F3 to equivalence nodes along the plane of symmetry
-I assume the 'Bottom plate' is attached to the ground so it was constrained with SPC in all DOF.
-contact is set as surface to surface (DISCRET=S2S)
-contact stabilization CNTSTB were defined and referenced in the subcase
-nonlinear expert system was activated PARAM>EXPERTNL>YES
-Nonlinear Monitoring was activated PARAM>NLMON>DISP
-the number of increments was increased to 3 in the NLPARM>NINC=3

Unable to find an attachment - read this blog

Rod

Glad to help.

Yes, usually models experience convergence difficulties if they are not properly constrained. This is especially problematic with models constrained only by contact.

The following changes were made to make the model converge:
-the main issue was that the girder was split at the midpoint. Shift+F3 to equivalence nodes along the plane of symmetry
-I assume the 'Bottom plate' is attached to the ground so it was constrained with SPC in all DOF.
-contact is set as surface to surface (DISCRET=S2S)
-contact stabilization CNTSTB were defined and referenced in the subcase
-nonlinear expert system was activated PARAM>EXPERTNL>YES
-Nonlinear Monitoring was activated PARAM>NLMON>DISP
-the number of increments was increased to 3 in the NLPARM>NINC=3

Thanks a lot Hyperman.

The bottom plate won't touch the ground when the loading beam will be moved up. This is the case I am analyzing.

I deleted the supports attached to the bottom plate, run and still the solution doesn't converge.

Unable to find an attachment - read this blog

Simon Križnik

You're welcome.

If the structure is only supported by contact at both ends of the girder, then the towers will undergo rigid body motion (rotation) after 70% load increment causing convergence difficulties for implicit method. This can be observed in the *_nl.h3d bellow (activated by PARAM>NLMON>DISP).

<?xml version="1.0" encoding="UTF-8"?>

You mentioned the girder is supposed to move up, but in the shared models there are only downward forces acting on the top of both towers. Also, if the structure is initially on the ground, the outermost edge of the towers baseplate will slide on the ground during rotation, as indicated by the undeformed plot.

I have converted the Optistruct model to Radioss, because the explicit method does not fail due to rigid body motion. Note that the 'dummy' material was assigned a density of steel due to the timestep issue, therefore the model is heavier (77 instead of 38 tonnes). The same rotation could be observed indicating the towers are not properly constrained, so boundary condition assumptions should probably be revised.

<?xml version="1.0" encoding="UTF-8"?>

Unable to find an attachment - read this blog

Rod

You're welcome.

If the structure is only supported by contact at both ends of the girder, then the towers will undergo rigid body motion (rotation) after 70% load increment causing convergence difficulties for implicit method. This can be observed in the *_nl.h3d bellow (activated by PARAM>NLMON>DISP).

<?xml version="1.0" encoding="UTF-8"?>

You mentioned the girder is supposed to move up, but in the shared models there are only downward forces acting on the top of both towers. Also, if the structure is initially on the ground, the outermost edge of the towers baseplate will slide on the ground during rotation, as indicated by the undeformed plot.

I have converted the Optistruct model to Radioss, because the explicit method does not fail due to rigid body motion. Note that the 'dummy' material was assigned a density of steel due to the timestep issue, therefore the model is heavier (77 instead of 38 tonnes). The same rotation could be observed indicating the towers are not properly constrained, so boundary condition assumptions should probably be revised.

<?xml version="1.0" encoding="UTF-8"?>

Thanks a lot Hyperman! Your replies were extremely helpful and well explained. You just saved my ass.

How i wish all replies will be like this. Kudos to you bro!

Unable to find an attachment - read this blog