Cancel
Showing results for 
Search instead for 
Did you mean: 

Problem with Advanced Nonlinear Static (unstable model)

Creator
Creator

Hi, Dear All

I am a FEMAP beginner user.

 

Kindly please help me to find a solution of the issue I had faced.

I want to analise the model shown below

01.jpg

 

 

Model have 8 connectors: 5 real contacts (Initial penetration - 2.Calculated/Zero Penetration)

and 3 contacts with gap (gap betwen bolt and holes in the sphere and wachers) - Initial penetration - 3.Zero Gap/Penetration.

 

02.jpg

 

 

When I use analysis type linear static I dont have  problems

 

03.jpg

 

But I want to get a result for the model in which the nonlinearity of the material is taken into account

(analysis type - 22..Advanced Nonlinear Static)

 

In this case, at the beginning of the calculation, I get a message stating that the model may not be stable. After about 10 minutes of calculation, I get a message about a fatal error.

05.jpg

What advice can you give? How to change the model?

My model is attached below


Thank you in advance

6 REPLIES

Re: Problem with Advanced Nonlinear Static (unstable model)

Siemens Phenom Siemens Phenom
Siemens Phenom

I think there is a problem with your material model.  You specify a very high yield stess in comparison to what you show as a yield stress in your Stress vs. Strain function.  When I switch the material to a elastic material, the model converges quickly in Advanced Nonlinear Statics.

Best Regards,
Chip Fricke
Principal Applications Engineer - Femap Product Development

Re: Problem with Advanced Nonlinear Static (unstable model)

Creator
Creator

Dear, Chip Fricke.
Thank you very much for your answer.

Re: Problem with Advanced Nonlinear Static (unstable model)

Creator
Creator

Hi

I continue to solve the problem described above. I have a few questions. If you have any thoughts or solutions, please respond.

In the corrected model  (The model is attached at the end of the repost)  for all elements assigned:   nonlinearity type - "none". 

Except material for the bolt and nuts for which the property is assigned: nonlinearity type - nonlinear elastic with function "bolt and nuts - vs stress".

001.jpg

problem 1.

For the calculation of type 22 Advanced Nonlinear Static, I obtained a linear dependences of the nodes, but in a real experiment I obtained nonlinear dependences. Perhaps I do not understand the calculation algorithm for nonlinearity type - nonlinear elastic. 

002.png.jpg

Question for problem 1: Is it possible in my model to obtain a nonlinear dependence for deformations (calculation with a real deformation diagram for a bolt and nut material).

My experimental data are nonlinear dependencies. By results of calculation in FEMAP linear

03.JPG

I thought the problem could be solved if I switch nonlinearity type, but in this case I got a new problem.

 

problem 2: 

When i switch the nonlinearity type - nonlinear elastict to plastic with function "bolt and nuts - vs stress" 

During the calculation, I get a message about a fatal error. I tried to solve this problem in two ways: 1) - reduce the load; 2) change the function so that the maximum stress on the diagram is greater than the stress that I received in the elements of the model during the static calculation. But these methods do not solve the problem.

 

 

Re: Problem with Advanced Nonlinear Static (unstable model)

Siemens Phenom Siemens Phenom
Siemens Phenom

I believe the issue with the plastic material run is  in the iteration settings. I turned on line search as shown below after setting the bolt and nuts material to plastic and useing function 3 for the stress/strain curve.

2017-08-02 16_21_02-NASTRAN NXSTRAT Iteration and Convergence Parameters.png

 

This runs to completion and elements follow the stress strain curve as expected, see the results sample below:

2017-08-02 16_19_46-Femap with NX Nastran - [m20.modfem _ Linear Displ].png

 

Regards,

 

Joe

Re: Problem with Advanced Nonlinear Static (unstable model)

Creator
Creator

Joe many thanks for your reply.
Tell me what and where should I change in the settings to
The model looked like in your post on the picture 2 (zone 1 , 2 ).
P.s. I will be very proud of you if you find the time to attach a file with your changes

011.JPG

 

Re: Problem with Advanced Nonlinear Static (unstable model)

Siemens Phenom Siemens Phenom
Siemens Phenom

To set the view of the bolt only with the legend values using only that material try the following:

Use Group/Operations/Generate Material( this will make a group for each material)

Using Visibility( I use Model info tree); RMB on Group; choose "show active group" then make sure active group is material 2

Next in Post processing toolbox set the 2 highlighted options shown below:

2017-08-03 10_01_33-Femap with NX Nastran - [m20.modfem] - [Linear Displ].png

 

The chart to show the nonlinear behavior matching the input stress/strain curve; use the vector vs vector option to create a data series for an element of interest, then create another data series using the function for the stress strain curve.

 

Regards,

 

Joe