*** 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
There is at least 1 small equation solver pivot term plz help!!
- 1.9K Views
- Last Post 30 December 2019
- Topic Is Solved
*** ERROR *** CP = 1.469 TIME= 230:45
Some part of the model is free to rotate about the Y axis. Add a constraint to stop that.
How many parts are in this model and how are they connected to each other? How is the model connected to ground?
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 !!??
In Mechancial, under Static Structural click on Analysis Settings. Large Deflection is turned on there.
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
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
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.
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
i try every member and no thing !!!?
please help !!!
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.
that's what i figure out and fixed unless one member can't find
*** 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
can't find that element !!!!
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.
i try simple model and nothing, same error
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.
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?
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, please open a New Discussion to ask this question, and perhaps add some detail about what you are trying to accomplish.
- All Categories
- Community Rules, Guidelines, and Tips
- News & Announcements
- Student Products
- Pre and Post Processing
- Tutorials, Articles and Textbooks
- Installation and Licensing
- Physics Simulation
- Student Competition Teams
- eMasters Degree from UPM
- Site Feedback