Altair RISE

A program to recognize and reward our most engaged community members

Nominate Yourself Now!

Contact Definition & ERR99%

Greetings!

I'm currently facing an issue in my simulation where the error rate fluctuates drastically from 0% to 99% in an instant, just after the start (run it and you'll see). Despite experimenting with various approaches and having successfully run similar simulations before, I've been struggling with this particular issue for over a week without any progress. While I'm not particularly skilled in Radioss, I'm considering the possibility that the problem might lie in the contact definitions. I did manage to get the simulation to run properly once by adjusting Gapmin, which leads me to question whether it's configured correctly. Though, I've followed the same reasoning as in others with succesful results. Here are the considerations I've made for Gapmin:

- Contact Crash - Barr: The distance between the shell and the closer node of the crashbox.
- Contact Crash - AIP: Half of the combined thickness of each.
- Contact FBH - AIP: Half of the AIP thickness. (FBH is a composite, and theoretically, I've set the surface as the upper layer of the laminate by setting Ipos=3 after reviewing normals).

Any insights or suggestions you might have would be immensely helpful. Thank you in advance!

cat14x_v2.hm

Find more posts tagged with

English

Radioss

Accepted answers

Polyvios Romanidis

Hi Albert,

I have some general improvements to propose in your model, some of them might be critical for the errors you get.

In Shell Property you can set N=0, because no other set up is compatible with /MAT/LAW1.
I think that you should re-mesh the part with ID=8 because elements in the flange have great differences in the size. It is preferable to have even some /TRIA elements instead of having great element size differences.
In /INTER/TYPE2 you can just leave the flange nodes from your part with ID=8, If you check out in 0.out file all the other 1722 nodes are removed either way from your interface.
For the Interface with ID=1, it is more suitable to insert Gap_min value equal to 0.42 (half the thickness of the part) and also insert an Inacti = 6 formulation.
I see that the part with ID=6 have a thickness greater of 20 mm and this caused mainly by a specific layer of 20mm thickness itself. I think that you probably try to simulate a honeycomb layer there, but this is not recommended to be done with shell elements. This can cause problems both with interfaces, because of the great thickness, and with material behavior, which can not be done generally with 2D elements for Honeycomb structures. Also you have not define a specific plastic behavior for the material of this layer, so if the yield point reached you might have some problems.

I would say that mainly points 4,5 are critical for the strange behavior you are getting. The first 3 points will help you just to have a more clear model.

It is a good idea to firstly set up your model without composite materials and instead use /MAT/LAW2 and /PROP/SHELL, just to check the interfaces set up. Then try to implement the composites to be sure that everything else works and, if you have to set honeycomb structure, prefer a shell-solid-shell element set up to have a proper defined model.

Polyvios

All comments

Polyvios Romanidis

Hi Albert,

I have some general improvements to propose in your model, some of them might be critical for the errors you get.

In Shell Property you can set N=0, because no other set up is compatible with /MAT/LAW1.
I think that you should re-mesh the part with ID=8 because elements in the flange have great differences in the size. It is preferable to have even some /TRIA elements instead of having great element size differences.
In /INTER/TYPE2 you can just leave the flange nodes from your part with ID=8, If you check out in 0.out file all the other 1722 nodes are removed either way from your interface.
For the Interface with ID=1, it is more suitable to insert Gap_min value equal to 0.42 (half the thickness of the part) and also insert an Inacti = 6 formulation.
I see that the part with ID=6 have a thickness greater of 20 mm and this caused mainly by a specific layer of 20mm thickness itself. I think that you probably try to simulate a honeycomb layer there, but this is not recommended to be done with shell elements. This can cause problems both with interfaces, because of the great thickness, and with material behavior, which can not be done generally with 2D elements for Honeycomb structures. Also you have not define a specific plastic behavior for the material of this layer, so if the yield point reached you might have some problems.

I would say that mainly points 4,5 are critical for the strange behavior you are getting. The first 3 points will help you just to have a more clear model.

Polyvios

Albert Grima

Hi Albert,

I have some general improvements to propose in your model, some of them might be critical for the errors you get.

In Shell Property you can set N=0, because no other set up is compatible with /MAT/LAW1.

I think that you should re-mesh the part with ID=8 because elements in the flange have great differences in the size. It is preferable to have even some /TRIA elements instead of having great element size differences.

In /INTER/TYPE2 you can just leave the flange nodes from your part with ID=8, If you check out in 0.out file all the other 1722 nodes are removed either way from your interface.

For the Interface with ID=1, it is more suitable to insert Gap_min value equal to 0.42 (half the thickness of the part) and also insert an Inacti = 6 formulation.

I see that the part with ID=6 have a thickness greater of 20 mm and this caused mainly by a specific layer of 20mm thickness itself. I think that you probably try to simulate a honeycomb layer there, but this is not recommended to be done with shell elements. This can cause problems both with interfaces, because of the great thickness, and with material behavior, which can not be done generally with 2D elements for Honeycomb structures. Also you have not define a specific plastic behavior for the material of this layer, so if the yield point reached you might have some problems.

I would say that mainly points 4,5 are critical for the strange behavior you are getting. The first 3 points will help you just to have a more clear model.

It is a good idea to firstly set up your model without composite materials and instead use /MAT/LAW2 and /PROP/SHELL, just to check the interfaces set up. Then try to implement the composites to be sure that everything else works and, if you have to set honeycomb structure, prefer a shell-solid-shell element set up to have a proper defined model.

Polyvios

Hello,

Indeed, it was point number 5 that was causing the issue. After deleting the ply and creating it again, the error no longer occurs. As a result, I'll follow the recommendation to simulate with the solid core.

Thank you very much for your help!