Error 1241: error in property
Hello,
I am currently working with Hyperworks Desktop v2017.3 and RADIOSS solver v2018. I am using MAT LAW 93 (ORTH_HILL) which can be used with PROP TYPE 51 as mentioned in the reference guide for RADIOSS solver. Accordingly, I setup a model with the above mentioned MAT and assigned the created plies and laminate to the PROP. I am attaching the .rad file for reference. When I tried to run the model, it gave error saying 'SHELL ELEMENT ID: 100004353 DOESN'T BELONG TO ANY PLY. MAY BE IS NOT THE ONLY SHELL ELEMENT WITH THE SAME ISSUE'. I don't understand how to resolve this issue. Kindly help me.
Thanks,
Madhura
Answers
-
hi
It seems you are referring the laminate property id 1 inside it self.
Maybe you need to use the property id 3, ply, instead.
Regards
0 -
Hello,
Your application is composite forming isn't it?If so, some suggestions :
0- As Rogerio says, your property TYPE51 used the ply id 1 that is not referenced and call itself
1- Prop TYPE51 need to be define for only 1 part, in your case 2 properties for the 2 plies
2- In case of forming simulation this property is used to modeled fiber with /MAT/LAW58 (FABR_A) in addition to hyperelastic law for the matrix if needed
3- This error comes from the ADMESH parameter which is not used for composites due to the SMP restriction. Better to use the refinement mesh at the start of the study. To avoid this error, you must remove this setting.
This is answering to your question?
Best regards,
Arthur
0 -
I have the same error , althought i assign my plies to all elements of the component windshield " pare brise " , but the error is shown all time .
here is my file attached to check it if it's possible
0 -
Mehdi_21989 said:
I have the same error , althought i assign my plies to all elements of the component windshield " pare brise " , but the error is shown all time .
here is my file attached to check it if it's possible
Hi
It seems that you do not have an /STACK defined on the model.
In HyperMesh, when you create the laminate, define the cardimage=LAM_STACK. So that /STACK will be defined.
It is suggested running the model checked in Hypermesh (Tools > Model checker) that will help you debug the model.
Also, you need to define material to the component (/PART), and /GRAV is missing the /FUNCT.
Let us know that this is helpful.
Regards
0 -
Rogerio Nakano_21179 said:
Hi
It seems that you do not have an /STACK defined on the model.
In HyperMesh, when you create the laminate, define the cardimage=LAM_STACK. So that /STACK will be defined.
It is suggested running the model checked in Hypermesh (Tools > Model checker) that will help you debug the model.
Also, you need to define material to the component (/PART), and /GRAV is missing the /FUNCT.
Let us know that this is helpful.
Regards
Hi sir , thank you first for your reply ,
- i have created on my model the stack , but solver shows error that materials law 1 and 2 ( elastic mat and plasticity Johnson cook ) aren't compatible with stack .
- i can't define a material for my part (winshield) because it is the composite which materials are defined by default in the laminate stack .
0 -
Mehdi_21989 said:
Hi sir , thank you first for your reply ,
- i have created on my model the stack , but solver shows error that materials law 1 and 2 ( elastic mat and plasticity Johnson cook ) aren't compatible with stack .
- i can't define a material for my part (winshield) because it is the composite which materials are defined by default in the laminate stack .
Hi
1- You can check in the Documentation the material law that is compatible with /PROP/PCOMPP
2- You need to define a material for the /PART.
Material referred to in the /PART card is used only for calculation of time step and contact stiffness.
Regards
0
Altair Employee