ERROR ID :54 ** ERROR IN INPUT FORMAT

Jeugarcon

Hello,

I created a model of a curved beam with two extremities free of rotation in loading plane (XY plane), the right extremity is applied with an initial velocity. So I made the two extremities rigid bodies, but it has thousands of errors when compilation: "ERROR ID :54  ** ERROR IN INPUT FORMAT  IN BLOCK:.......".

I checked this type of error in this forum, according to the answers, I tried Model Checker-Auto correction, and updated the elem types. But there exists the same errors when submitting calculation. 

In this post: https://community.altair.com/community?id=community_question&sys_id=3f560cf61b2bd0908017dc61ec4bcbb0, someone said maybe the problem is with the rigid body, I have the same warning mentioned in this post:"Rbody ID is different from master ID".

Could someone help me solve this problem? Any help would be appreciated. (The starter and engine files are attached)

Best

Rodrigo Merigo_22161

Hi!

It looks like the error is related to the solver deck itself rather than the model settings. Are you running Radioss version 14? If you have any other versions available you could try exporting the deck for those versions as well. I imported your model in HyperMesh and exported again, now it seems to finish the starter sucessfully. Please try the model attached.

Thanks.

 

Jeugarcon

Rodrigo Merigo_22161 said:

Hi!

It looks like the error is related to the solver deck itself rather than the model settings. Are you running Radioss version 14? If you have any other versions available you could try exporting the deck for those versions as well. I imported your model in HyperMesh and exported again, now it seems to finish the starter sucessfully. Please try the model attached.

Thanks.

 

Hello Rodrigo Merigo,

Thanks for your reply, actually, I am using Radioss version 14, your attached file can be compiled now. It is strange if you did no modification about my model...

Indeed, I also tried to delete the rigids in my model, it works when compiling, so maybe the setting of "rigids" does have something wrong.

Best

Simon Križnik

Hi,

 

the error is due to rigid elements in the same component as shell elements of extremity 1&2 components. This is invalid: only elements of the same type are allowed in a component. Furthermore, the rigid elements should be placed in a separate component with PART card image with RBODY option, but without property and material reference. The rigid outputblocks were also revised.

 

Jeugarcon

Simon Križnik,

Thank you for your detailed explanations, that really helps! I understand where the problem is.

Now I have rigid elements in isolated components, but now I don't understand what's the function of "extremity 1&2" components in my model? Can they be deleted? Because I want to suppose that the two extremities are rigid bodies, "extremity 1" is free in dof1&6, and "extremity 2" is free in dof6. In addition, for the interface between "body" component and extremities, which one is right(interface between "body" and "extremity 1&2" or interface between "body" and "RigidBody")?

Thank you in advance.

Best

 

 

Simon Križnik

Elements of Extremity 1&2 components should not be deleted, because their mass is still involved and its elements can be used in the contact interface. It is important to set realistic material properties for components made inflexible by a rigid element because contact stiffness is calculated based on material properties.

 

The contact interface should be defined between "body" and "extremity 1&2". 

 

 

Jeugarcon

Hello ,

It is grateful for your helpful explanations! That really helps!

 

Best

 

Jeugarcon

Hello,

When I put an imposed velocity on primary node of rigid body, there is no strain value after calculation in Hyperview as if there is no loading. But when I put an initial velocity on the same primary node, it works. What is the problem? The files are attached. Thanks.

 

Best

 

 

Simon Križnik

Hi,

 

the problem is you have assigned a material law 13 to extremity 1&2. MAT/RIGID is obsolete and is not compatible with /PLOAD, /CLOAD, /GRAV, /IMPDISP, /IMPVEL, /IMPACC, /IMPTEMP, /INIVEL and /INITEMP. Instead, use any other valid material model. Also, check unit consistency- you have declared kg, m, s units in the BEGIN_CARD, but you have materials that span a density range of three orders of magnitude.

 

I have also activated advanced mass scaling to speed up computation.

Jeugarcon

Hello,

Yes, material law 13 is invalid when using /IMPVEL, now it works.

Thank you very much!

 

Best