There is at least 1 small equation solver pivot term plz help!!

  • 119 Views
  • Last Post 3 weeks ago
  • Topic Is Solved
mohammed164 posted this 21 October 2019

*** 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.                                                     

Attached Files

Order By: Standard | Newest | Votes
peteroznewman posted this 22 October 2019

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

  • Liked by
  • mohammed164
mohammed164 posted this 5 weeks ago

i'm sorry but how !!?

peteroznewman posted this 5 weeks ago

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

  • Liked by
  • mohammed164
mohammed164 posted this 5 weeks ago

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 posted this 5 weeks ago

peteroznewman posted this 5 weeks ago

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

  • Liked by
  • mohammed164
mohammed164 posted this 5 weeks ago

THANKS AGAIN 

mohammed164 posted this 4 weeks ago

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 posted this 4 weeks ago

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.

  • Liked by
  • mohammed164
mohammed164 posted this 4 weeks ago

Is it possible to have error because zero member?

mohammed164 posted this 4 weeks ago

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 posted this 4 weeks ago

What is a zero member?

mohammed164 posted this 4 weeks ago

 

like this !

no force, no tension, no Compression

mohammed164 posted this 4 weeks ago

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

mohammed164 posted this 4 weeks ago

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 posted this 4 weeks ago

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.

  • Liked by
  • mohammed164
mohammed164 posted this 4 weeks ago

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

 

mohammed164 posted this 4 weeks ago

*** 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 !!!!

Attached Files

peteroznewman posted this 4 weeks ago

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 posted this 4 weeks ago

i try simple model and nothing, same error

i'm disappointment  

mohammed164 posted this 4 weeks ago

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

peteroznewman posted this 4 weeks ago

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 posted this 3 weeks ago

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 posted this 3 weeks ago

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.

Close