Edge to edge surface contact separation in Non Linear Analysis

[s_k_alfonzo]

Hello All,  

I was hoping I could get some guidance as to what is going on with this Non-Linear outcome. 

I have this 20.6-meter-long x 1.6 meter tall I beam. Simply supported (Pin connection at left end and translation allowed at the right end-see attached fig.1). Also I have added frictionless constraints every 4 flanges to avoid displacement in the Z direction (The FEMAP example I am following uses  bracing but I am not sure if you can do that in Inventor/Nastran,  however I think frictionless is doing the same function). A distributed load of 130 kN/m is supposed to be added but distributed loads seem to be an issue with Nastran so a total load of 2600 kN was added (through the entire beam length- applied on the mid chord). 

 

 The material I have defined is type: Elasto-Plastic (Bi-linear). Initial Yield Stress: 235 Mpa. Youngs Modulus: 2.1E+11 (Pa). 

 A couple of notes: 

1. The model is assembled by a series of short surfaces, rather than a typical long top and bottom flange, and 1 long web (fig.2 attached for clarification)  

    

2.  I have defined contact as surface contact and checked "Specify Contact Regions" selecting the entire structure. See Fig.3 (before defining contact like this the analysis would not work at all, even running a Linear Static Solution) 

 

3. Prior to running the Non-Linear Analysis, I ran a Linear Static one just to see if the model was stable. The analysis ran (see fig. 4). There are no surfaces separating at any point and the displacement outcome is similar to what I am supposed to obtain in the Non-Linear Analysis (judging by the results obtained in FEMAP ~1.4 meters, max. displacement) 

4. I ran the Non-Linear Analysis with the following settings:  

1. Type: Non-Linear Static 
2. Contact type: Bonded. Tolerance: 0.0001 
3. Large displacements: off 
4. Increments: 30 
5. Non Linear material as defined above

MAIN QUESTION:

Why do surfaces separate in the non linear analysis whereas the linear analysis seems to deformed properly? (see fig.4, fig. 5 and fig.6 )

Fig. 4 Linear Analysis - Displacement outcome

fig. 5 Non Linear Analysis

Fig. 6 Non Linear Analysis - Close up

 

 

[John_Holtz]

Hi @s_k_alfonzo  Welcome to the Inventor Nastran forum.

It will not be possible to answer your questions without having the model. Looking at images do not provide the answers to the questions that we have. (If the model is a single part file, you can attach the .ipt file to the forum post. If the model is an assembly, you need to create a pack-and-go file using the attached instructions and attach the .zip file to the forum post.)

Here are some comments/questions based on your description.

1. A displacement of 1.5 m is unbelievable. Please tell us that you are not designing a bridge, building, or other critical structure. 🙂
2. Bonded contact is the wrong type of contact for shell elements. Please use offset bonded contact so that the joints behave like continuous material (a welded joint) instead of hinge joints.
3. If you are using solver contact for the entire model, there is no reason to select the entire model. Leave the "Specify Contact Regions" unchecked.
4. You should be using "Continuous Meshing" checkbox on the Mesh Settings dialog so that all the edges are connected together by matching the nodes. There is no need to use any contact in the model. (However, sometimes the meshing does not work with continuous meshing, in which case contact is the solution.)
5. I suggest not using frictionless constraint when you can use a regular constraint and fix the Y direction. (I assume that you meant Y instead of Z. Although if you constrain the Z direction, that would fix the 1.5 m displacement!)

John

[s_k_alfonzo]

Hello John, 

Thank you for getting back to me. 

I fixed the surface separation issue by enabling continuous meshing. I also removed frictionless constraint. The analysis ran to completion at 100%. However, the final displacement doesn't match the expected result of approximately 1400 millimeters. 

I've reviewed the settings for the exercise multiple times but haven't been able to find the mistake. I'm hoping you can help me find what's wrong. 

Here's a summary of the settings I used: 

• Analysis type: Non-Linear Static 
• Material type: Elasto-Plastic (Bi-linear) 
• Initial Yield Stress: 235 Mega Pascals 
• Young's Modulus: 210,000,000,000 Pascals 
• Large displacements: OFF (as per the example setup) 
• Number of increments: 30 
• Load: 130 kN/m (applied as a total force of 2,600,000 Newtons, which is 130 kN/m times 20 meters for the beam's length). 

I've attached the model for your reference. (Assembly name: EFEA_03_010)

[John_Holtz]

Hi @s_k_alfonzo 

Is the description of the original example online somewhere? If so, can you provide a link? Or if you have the example in a format that can be posted to the forum, that would be helpful.

I suspect the material properties in your model do not match the example.

• With elastic material properties, the theoretical displacement is 73 mm. The linear static analysis matches that (76 mm) and shows that the entire flange thickness will yield between the stiffener plates, but not much more of the beam is above the yield stress.
• With the nonlinear properties entered, the tangent modulus (ET) after yielding = 0.1*modulus of elasticity. That is, the portion that yields has 1/10 the original stiffness. If the entire beam were 1/10 the original stiffness, the displacement would be 10*73 = 730 mm. It is not possible for the model to reach 1400 mm displacement with the entered material properties. The actual displacement will be much smaller than 730 mm since only a small volume of the model is yielding. (Nastran calculates 115 mm.)

As the tangent modulus (ET) becomes smaller, the displacement will increase. But the beam becomes less stable, so the analysis may have difficulty converging.

John