I am attempting to do a simple plate deformation analysis using the advanced nonlinear analysis. I went through the Femap example before but I am not having any success with my plate deformation model.
I am not sure if I am missing anathing or if I need to increase the number of iterations that are needed to converge. Any help on this would be much appreciated.
For the Advanced Nonlinear solver, you should use a Function of type Time to apply the loads as shown below.
However, there is another major issue with the model you attached in that the Connection Regions do have have continuous element faces assigned. The first model I've attached cleans that up by using surfaces to define the regions. Note that Femap v11.3 has a much improved interface to select adjacent element faces that will make this operation faster and more robust.
The results using the change to the model as outlined above are shown here.
Additional comments I have are that the element aspect ratios are greater than 10:1 for all of your solid tetrahedral elments plus you only use one element thick across each of the two plates. This will result in inaccurate results for bending. For parabolic solid tetrahedral elements, you need at least two elements across the thickness where bending occurs and more where there are high stress gradients, you'll need more to get accurate results.
Since this model lends itself well to hex meshing, I've attached a sample model using four (4) hex elements across each plate.
Also, this could be modeled using plate elements instead of solids, especially if you do not need to see the stress gradiant across the thickness of the plate(s). Is this model a test model to see how to set up an Advanced Nonlinear analysis, or representative of what need to perform as part of your work?
Thank you for the help. I really appreciate it.
This was purely a test model to evaluate the contact capabilities of Femap since I am new to Femap.
The element aspect ratios aren't refined since I wanted a quick run to check if the model works or not.
As for establishing the contact regions using surface, I tried it. However for some reason when I got the results the surfaces penetrated each other (which I suspect the mesh was not associated with the surface). I am not sure how it happened but if there is a way to link the mesh to geometry please let me know.
For version 11.3, I would like to suggest the following:
1) When I run multiple load cases and view the results in post-processing, as I toggle between the analysis cases, the applied loads do not change.
Let's say Analysis 1 was for Load Case 1, and the results are in Output 1.
Analysis 2 was for Load Case 2, and the results are in Output 2.
When I load the contour plots to view results in Output 1, the applied load would show Load Case 2 since that is active Load Case. Although it is only a visualization issue, when I view Output 1, Load Case 1 should automatically become the active Load Case.
The likely reason why Femap does not automatically match the load set with the output set is because the output set can often be created without direct reference to a matching load set. For example, when setting up a multi-case analysis in the Analysis Manager, the cases can be eg. linear combinations of other individual cases (Ie. SUBCOM instead of Standard Case), so the output does not have a direct connection with a specific load set.
I am not sure that the output data in the NX Nastran OP2 file has any way of storing that "link" information. So yes, for simple load / analysis cases it would be nice if the load set could be "attached / linked" to its equivalent Analysis Case & Output Set, but the general capability is that NX Nastran Output sets (even in linear analysis) are not always produced through a direct matching Femap load set.
Thank you so much for your help.
If I don't input the load as a function of time, will the non-linear analysis not work.
Furthermore, if I wanted to run another load case to simulate the unloading case and view residual streeses how do I go about doing that. For linear analysis I could stack up different subcases in one Analysis set.
I want to set up some friction betwwen the contacting plates. I go to the connectors property and select the NX advance nonlinear tab. On the right side in friction model I select default and input the coefficient of friction in Friction Param 1. Then what is the frictional constraint parameter and friction delay.
When I have two bodies in contact, I am trying to ensure that the nodes and elements on the contacting faces match up to get a faster solution. In this case the geometries are quite simple so it is easy for the nodes to match up. However for contacts involving complex geometry is there any way to match up the mesh between contacting surfaces. I tried partitioning the bodies so both bodies have same surfaces in contact. However this does not work out in certain cases. If there any any best practices please share them.
Thank you in advance for all your help. As a new user I really appreciate the help.