Issues with contact in NL static simulation

[Anonymous]

Hello!

setup

I'm working on a project where I'm deforming a hyperelastic frame in different ways and matching it against a prototype to determine which simulation is most valid. I've already done one where I pull the frame down from the top edges using enforced motion, and am working on a contact based one where the frame is pressed against a flat plate(see the setup on the left). So far I've been able to get it to solve, but there are some oddities with the solution that make me question it's accuracy.

The solutions that solve keep a gap between the surface and the tip of the "flap" on the frame. This makes me think that I improperly configured the contact settings. The contact settings currently are between the bottom of the plate and all top faces of the frame (from the round tip of the flat to the fillet on the right side of the top of the frame). Furthermore, the flap barely deforms and the part with ridges never even gets close to the top of the plate, while on the physical model it lies almost flat with the plate. While the SPC summation of forces almost match in the models, unfortunately part of the design criteria involve aesthetics so the accuracy of the deformed shape is very important.

While attempting to modify the contact settings, I've encountered 3 different situations (excluding errors). The first is that the bottom face will buckle without any load being transferred to the rest of the frame. Secondly, the frame will traverse the gap and impact the plate. At this point the load gets transferred to the plate in a non-uniform fashion though 3 or so "hotspots". Lastly, the gap will remain but the frame will fold as designed.

I feel like I've missed something pretty obvious, and any help would be appreciated! Let me know what other information I can provide to help you diagnose the issue.

[John_Holtz]

Hi @Anonymous . Welcome to the Inventor Nastran forum.

It would be best if you could attach the model and let us know what version you are using. That way, readers that have the same version (or newer) can open the model and get a better understanding about what is occurring.

Here are the steps to create a pack-and-go file of the Inventor model. (The Nastran input is saved in the part or assembly file.) Attach the zip file to your forum post.

Based on the video by Roelof Feijen

1. “File > Save As > Pack and Go”
2. Specify the Destination Folder. Specify a new folder (or an empty folder) such as “C:\Nastran model\Project ABC”.
3. Set the following “Options”:
   1. “Keep Folder Hierarchy”
   2. “Model files Only”
   3. Check “Skip Styles”
   4. Check “Skip Templates”
   5. Check “Package as .zip”.
4. Click “Search Now”. The “Files Found” list will give all the assembly (.iam) and part (.ipt) files used in the model.
5. Click “Start” to copy the files to the Destination Folder and zip them.
6. Click “Done” to close the Pack and Go dialog.
7. The parent folder of the Destination Folder will include the .zip file. The zip file will have the name of the destination folder. For example, “C:\Nastran model” would have a file named “Project ABC.zip”. “Project ABC.zip” would include all the Inventor files so that other users can open the model.
8. Indicate what file to open; that is, what is the name of the assembly or part file to open.

[Anonymous]

Alright, I've attached what I got out of it. And I'm using the 2020 version of Inventor Nastran.

[John_Holtz · Accepted solution]

Hi,

Here are my suggestions. Note that I used Inventor 2022 (because I had other things open at the same time) and cut the model to be be 0.23 inches deep instead of the original depth of Z inches (to make a smaller model that runs faster).

1. Remove the gap between the gasket and the glass. It is difficult to move a part that has no resistance in a static analysis. (Due to the gap, the gasket can be moved without force until it comes into contact with the glass. )
2. Set the friction to 0. That may have something to do with preventing the "flapper" from bending over so that the ridges come into contact with the glass. (My first run reached 100% without too much problem, but the flapper was not bending over as you experienced in one of your runs. With the friction set to 0, it is working better. Or maybe removing the gap between the parts is making it run better.)
3. Reset the parameters. I noticed that you had a couple of NLK...whatever set, probably because the model was not stable due to the gap between the parts. The artificial stiffness added through the parameters was preventing the gap between the ridges and glass from decreasing.
4. For the contact, switch the faces in the "master/primary" and "slave/secondary". (Click the button that switches which faces are in which selection box.) Then set the Penetration Type to unsymmetric. (Both of these are related to having a weak material gasket contact a stiff material glass. You want the weaker material in the slave/secondary set.) I also suggest setting the Maximum Activation Distance to minimize the number of contact elements created. I am trying 0.3 inch, but that may be too small now that the "flapper" is moving.
5. For the Nonlinear Setup, use 25 steps minimum. When left blank, the software tries to manage the number of steps, but it may try to make them too large and have problems converging.

The analysis is trying to run. I hope I did not make my contact Maximum Activation Distance too small for the amount of motion of the "flapper".

[Anonymous · Accepted solution]

Thank you so much for your help. I've taken most of your suggestions and then did some other stuff to help it converge. Just for anyone else who ends up with a similar issue in the future:

• Suggestions 1 and 4 were crucial to solving the issue, and resetting both NLKDiagAFact and NLKDiagMinAFact to 0 were also very important (I kept some parameters edited like NProcessors and Bisect). This was exactly the problem creating the gap.
• Reducing the width of the model was also helpful for increasing the speed of calculations, but introduced some convergence issues. These were solved by placing z symmetry constraints on each of the large faces (in essence, creating an infinite extrusion).
• The coefficient of friction was actually really important to the function of the model, without it the model would slide over to the left leaving the top right arm unstressed and the ridges not making contact at all. With it, it remains in place for the most part (exactly how the physical sample acts). For reference, I'm only using a coefficient of 0.05
• 0.3 in was totally enough for it to converge
• The time the more accurate model took to converge is significantly larger than the other model, so if you're looking for something quick, dirty, and less accurate, NLK parameters and a gap might be the way to go.

Thanks again!