Altair RISE

A program to recognize and reward our most engaged community members

Nominate Yourself Now!

Material assigment with composites in Radioss

Hi everyone,

I am currently working on a explicit simulation with composites in Radioss. I am using the material law M25_COMPOSH and assigning the component the PCOMPP property with the laminate. However I keep getting the error that the component has no material assigned.

Please, if someone can help I would be really grateful.

Thanks in advance

Find more posts tagged with

Radioss

v2025.1

Accepted answers

altair_fukuoka

I've found that some element does not have stress. It means that these elements does not have stiffness.

(#3481 has stress, but #3867 does not.)

I've checked that the element #3867 is surely used for all plies.

For me, it seems a bug. I wll report it to the development team and ask whether any workaround is there. Please wait just a little bit more。

altair_fukuoka

The simple fix is Ip=20 in your "/STACK",

If you would like to understand it deeply, could you please read the following explanation.

In your model, in the "/STACK", Ip=blank and Vx,Vy,Vz=blank,

In this case, the 1st material orientation projection vector is (1,0,0),

Since the normal vector of the many composite shell elements are (1,0,0), Radioss Starter should fail to projection. Starter should fail but passed anyway. I guess this is the cause.

In your model, the composite shell elements have Φs. I guess you want to define the material 1st direction by elemental coordinate system (N1-N2 orientation) and Φs rotation,

For this, you can use Ip=20,

All comments

altair_fukuoka

Hi,

Here is examples which I made. They are made of /MAT/LAW25 and /PROP/PCOMPP.

Even though it is written in japanese, I hope you can find the links to 7z files. These are examples.

I guess that you are missing the matarial ID in /PART. Even when using /PROP/PCOMPP, you need to input a charactaristic material ID in /PART,

Thanks,

image.png

altair_fukuoka

Sorry, I missed the link. Here is my example,

https://community.altair.com/discussion/60660/

Marc224

Hi,

First of all thank you for the response.

Yes, my problem is exactly that, in the /PART there is no material; because in every tutorial that I have been following, no one assigned a material.

Even if my laminate is made of several materials of LAW25 I just have to input one as a reference, right?

Thank you so much for your help.

Marc224

Hi,

When I assign a material of the laminate to the /PART, I get in the simulation that the body is not rigid enough as if it is just getting the properties of only one material and not the laminate.

Thanks

altair_fukuoka

Yes, it is used for time step and contact stiffness calculation.

https://2026.help.altair.com/2026/hwsolvers/rad/topics/solvers/rad/part_starter_r.htm

altair_fukuoka

I wonder if the laminate has only one ply. If true, the element does not have stiffness for bending and acts like as fabric sheet,

https://community.altair.com/discussion/37207/radioss-mat-law19-%E3%81%A8-prop-type9-%E3%81%A7%E3%81%A7%E3%81%8D%E3%82%8B-%E6%9C%80%E3%82%82%E5%8D%98%E7%B4%94%E3%81%AA%E5%B8%83%E3%81%AE%E8%A1%A8%E7%8F%BE

Marc224

Hi,

No my laminate is 4 plies of CFRP (/MAT/LAW25_COMPOSH), a 10mm thick structural foam (/MAT/LAW25_COMPOSH) and 4 plies of CFRP (/MAT/LAW25_COMPOSH). All of these plies are in the same laminate and share the property(PCOMPP). But when I simulate it, it just does not offer any rigidity and acts like a "sheet of paper" and in Radioss I cannot check the engineering constatns.

I have tried to simulate the same simulation with a 4mm aluminum sheet and it runs just fine. So the problem is in the laminate and its stiffness.

Thanks

altair_fukuoka

It is impossible for me to guess the reason.

Can you upload your model?

or, If you cannot upload your model, could you contact to your local official technical support with your model?

Marc224

CRASHTEST_V4.hm

Yes, here it is.

altair_fukuoka

I've found that some element does not have stress. It means that these elements does not have stiffness.

(#3481 has stress, but #3867 does not.)

I've checked that the element #3867 is surely used for all plies.

For me, it seems a bug. I wll report it to the development team and ask whether any workaround is there. Please wait just a little bit more。

altair_fukuoka

The simple fix is Ip=20 in your "/STACK",

If you would like to understand it deeply, could you please read the following explanation.

In your model, in the "/STACK", Ip=blank and Vx,Vy,Vz=blank,

In this case, the 1st material orientation projection vector is (1,0,0),

Since the normal vector of the many composite shell elements are (1,0,0), Radioss Starter should fail to projection. Starter should fail but passed anyway. I guess this is the cause.

In your model, the composite shell elements have Φs. I guess you want to define the material 1st direction by elemental coordinate system (N1-N2 orientation) and Φs rotation,

For this, you can use Ip=20,

Marc224

Yes, that was the problem. Now, it works properly and I can keep developing the model.

Thank you so much for your help. It was really helpful!