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
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.
When I use analysis type linear static I dont have problems
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.
What advice can you give? How to change the model?
My model is attached below
Thank you in advance
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.
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".
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.
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
I thought the problem could be solved if I switch nonlinearity type, but in this case I got a new problem.
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.
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.
This runs to completion and elements follow the stress strain curve as expected, see the results sample below:
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
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:
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.