Learning Forum

[mohammed164]

*** ERROR ***                           CP =       1.469   TIME= 230:45
 There is at least 1 small equation solver pivot term (e.g., at the ROTY
 degree of freedom of node 348).  Please check for an insufficiently    
 constrained model.                                                     

[peteroznewman]

Some part of the model is free to rotate about the Y axis.  Add a constraint to stop that.

[mohammed164]

i'm sorry but how !!?

[peteroznewman]

How many parts are in this model and how are they connected to each other?  How is the model connected to ground?

[mohammed164]

THANK YOU AGAIN 

IF you don't get upset!!

i have anther problem when i try to exchange line body from beam to truss he told switch to large deflection but in solver control can't find large deflection option !!??

THANK YOU 

   

[mohammed164]

[peteroznewman]

In Mechancial, under Static Structural click on Analysis Settings.  Large Deflection is turned on there.

[mohammed164]

THANKS AGAIN 

[mohammed164]

hi

when i change line body from beam to link/truss and solve, give me error 

 *** ERROR ***                           CP =       1.391   TIME= 22:05:43
 There are 105 small equation solver pivot terms (e.g., at the UY degree
 of freedom of node 304).  Please check for an insufficiently           
 constrained model

and when modified element size in mesh to 10 and solve he give me that error

 *** ERROR ***                           CP =       1.219   TIME= 22:10:58
 There are 24 small equation solver pivot terms (e.g., at the UY degree 
 of freedom of node 182).  Please check for an insufficiently           

 constrained model.   

please helpppppp!!!!! 

[peteroznewman]

You need to set the Element size to a number larger than the total height of the model so that there is only 1 element on each line body.  You only want one link element on each line.  If the line body represents a wire, then you might want to set the element to be tension only so that it doesn't carry any compressive force.

[mohammed164]

Is it possible to have error because zero member?

[mohammed164]

same error !!!

 *** ERROR ***                           CP =       1.219   TIME= 22:10:58
 There are 24 small equation solver pivot terms (e.g., at the UY degree 
 of freedom of node 182).  Please check for an insufficiently           

 constrained model.   

[peteroznewman]

What is a zero member?

[mohammed164]

 

like this !

no force, no tension, no Compression

[mohammed164]

Is it truss/link required to resolve custom settings ???

[mohammed164]

hi 

I figure out what the problem and solved Except one element give me error 

*** ERROR ***                           CP =       1.469   TIME= 22:420
 There are 1 small equation solver pivot terms (e.g., at the UZ degree  
 of freedom of node 47).  Please check for an insufficiently            
 constrained model.

i try every member and no thing !!!?

please help !!!

[peteroznewman]

What are these lines across the section? That looks like there is a node/vertex at that point. If those are all Truss elements, that is no good.  If those are Beam elements then it is okay.

[mohammed164]

that's what i figure out and fixed unless one member can't find

 

[mohammed164]

*** ERROR ***                           CP =       1.266   TIME= 22:24:46
 There is at least 1 small equation solver pivot term (e.g., at the UZ  
 degree of freedom of node 100).  Please check for an insufficiently    
 constrained model.  

THAT ERROR

can't find that element !!!!

[peteroznewman]

Add a Modal analysis to the Static Structural Model.  Drag and drop any Fixed Supports or zero Displacement BCs.  The offending part may reveal itself.

The text file you attached is not useful for finding the problem.

You can create a Named Selection to show which node is # 100.  That would be helpful.

[mohammed164]

i try simple model and nothing, same error

i'm disappointment  

[mohammed164]

node selection give me this element what wrong !!?? 

[peteroznewman]

Doing a simple model is an excellent idea.  The defect in the simple model above is a lack of diagonal members on each face of the cube. That means it is a mechanism that can collapse, not a structure.

Do an even simpler model: three line bodies that come from a common point, the origin, 0,0,0.  Line body X is along the X-axis and the other end is 1,0,0. Line body Y is along the Y axis and the other end is 0,1,0.  Line body Z is along the Z-axis and the other end is 0,0,1.  Make sure you have only one LINK180 element on each line body. Make sure you do a Mesh Merge for the three nodes at 0,0,0 so there is only one node there. An alternative to Mesh Merge is to use Shared Topology in SpaceClaim.  Apply a force to the origin vertex.  Select the three vertices at the unit distance and make them Simply Supported. That model should solve without fail.

[mohammed164]

i made simple model and solve without problem

when add a member cross with anther member give me same error 

 

how can i solve this problem?

 

[peteroznewman]

Do you have four links that meet at a point in the center?  Are those four links in a plane? That creates a problem because there is zero stiffness of the center point in and out of the plane.  Don't do that, it is not a truss.

If instead you have two diagonal links that don't connect in the center, but just pass by each other and reach corner to corner, then you have made triangular shapes that have stiffness.

[mohammed164]

Hi,

How I can make zero length in spring!?

[peteroznewman]

Mohammed164, please open a New Discussion to ask this question, and perhaps add some detail about what you are trying to accomplish.

[mohammed164]

Ok

Thanks

[Haddouch Ibrahim]

Hello everyone, I face a problem when I want to compute elastic properties of nanoscale RVE using material Desing SpceCleam, the error is figured in the screen bellow