Non-linear analysis with enforced motion / Model overlap during simulation

[Jayson.Angeles]

Hi,

I am working my way to learn and conduct non-linear analysis using inventor nastran. I am trying to use enforced motion in the analysis but can't seem to fix the model to successfully complete the calculations. I have only seen one example so far on doing non-linear analysis so I would like to ask if someone can have a look at what I am doing and give me insights on what fix can be done to successfully run this. 

Just a summary, I am trying to simulate a metal component moving into a model that would resemble a rubber / silicone gasket. Loaded it with an enforced motion of 5 mm. In my head this should be simple but then again I may be wrong. 

I also notice some overlap in the model during the simulation. Can anyone share their insights on why and how can this be eliminated? Please see below. 

In addition, if there are some non-linear static analysis that can be shared I would greatly appreciate it. 

 

Thank you,

[John_Holtz · Accepted solution]

Hi @Jayson.Angeles . Welcome to the Inventor Nastran forum.

I have some questions, some of which I have answered for the benefit of other readers, and suggestions for the analysis.

1. What version are you using? (Answer: 2022)
2. You mentioned one example. What example was it? (I'm guessing this tutorial since it includes all the key aspects that are used in your sample: Autodesk Inventor Nastran 2022 Help | Tutorial A1: Metal Forming Simulation Using Nonlinear Material....)
3. What are we looking at in the image you show? (Partial answer in the figure below.)
4. I changed the enforced motion from 50 mm to 5 mm, as you mentioned. (50 mm is 3 times larger than the height of the block, so that was just a typo on the input.)
5. I thought some of the penetration is due to the large difference in elastic modulus between the parts: Titanium with E=1.1E5 MPa and Silicone with E=3 MPa. Sometimes the round off accuracy with such a large discrepancy can be a problem. I changed the titanium to 1.1E3 which helped, then I noticed other problems.
6. The contact is set between face 1 on the titanium and face 2 on the silicone. The "penetration" shown in your image is between face 1 and 3 where no contact is defined! You need to add face 3 to the secondary selection box of the contact so that face 1 makes contact with faces 2 and 3.
7. Until you get the analysis to run, set the friction to 0. No need to make the analysis 5 times more difficult when you can't get it to run.
8. Why did you refine the mesh along the edge of the parts and not over the entire contact face? (I decided to just mesh the entire model with a 1 mm mesh size. You may want to put the refinement on the three faces that come into contact.)
9. Whenever possible, enter a Maximum Activation Distance for the contact. Letting Nastran decide what activation distance is appropriate is just a bad idea. Since you have 1 contact, you can enter the Maximum Activation Distance without too much effort. 🙂 See Tip #18 in the PDF document attached to my forum post Suggested Reading - Tips and Tricks on the Inventor Nastran forum to understand why 6 mm is a good choice for the Maximum Activation Distance.
10. I think the analysis will not get to 100% (5 mm vertical displacement). It looks to me that the part will buckle, and buckling is not a static solution. See Figure 2 and the attached animation.

Figure 1: Exploded view to make it easier to "see" the contact faces. (The real gap between the parts is 0 in the model.)

Figure 2: Maximum load before the analysis is going to fail to converge. Is the silicone trying to buckle? 

Let us know if you have any questions.

John

[Jayson.Angeles]

Hello John, 

I appreciate the quick response and looking into the model I was working on. I followed your advice and was able to run the model. As mentioned, I does not complete up to 100% for it seems the silicone buckles. Nevertheless, I was able to pick up key points to follow moving forward.

Thanks again,

Jayson