Shell Model Stress Plot - Poor Gradient

[kseminsky]

Running a static-structural analysis on a rather large plate weldment. I've modeled and meshed using the midplane and offset surfaces generator. All gaps formed due to this process I am running the contact solver for offset bonded condition. The mesh overall looks good, the model runs efficiently, and I get result plots. Reactions and applied loads balance out. The only warnings I get are G301# for some elements with poor mesh (469,000 elements, 131 warnings) which is acceptable. I am running Nastran 2024, Version 18.2.0.35.

Where I am having concern with the analysis is the gradient of the Von Mises plot. It is very "patchy". I would expect a smoother distribution of stress over the geometry with the simple loading that I am applying. See attached images. I am running a 1.75" mesh and refinement as needed in curious areas. I have now refined the global mesh from 2.5" to the 1.75", and the patchy quality did not improve. 

Also, I have some transitions of thin to thick splices. This is where we increase plate thickness for local strength by using complete joint penetration weld from the thinner to the thicker plate directly in line with one another. I have these modeled as different idealizations with appropriate thickness values. It is peculiar that there is very low stress right at the transition. Why would this be? 

One other note - Since I do not have node match force transition between idealization and using the contact solver, I run a contact plot set to a very low maximum value to see that all my plates are connected properly. This looks good in the model (set to 2in maximum activation distance). I am limited to 3 attachments, so I will add the contact plot in a separate post. 

Open to thoughts, and I very much appreciate any input! Thank you!

@John_Holtz 

[kseminsky]

Adding the contact stress plot here. 

[kseminsky]

Bump

[John_Holtz]

Hi @kseminsky 

First, a question for the Inventor modeling experts. Is there a way to create a surface model that has N faces but one surface body, instead of N surface bodies with 1 face in each body? For modeling shells in Nastran, it would be better to have 1 surface body with 3 faces instead of 3 bodies. For a flat plate like this example, it is easy to split faces. For 3D structures, I do not know how to put all the surfaces into one surface body.

Figure 1: Three surface bodies require contact between the bodies. See attached "flat plate.ipt".

Both of kseminsky's questions are related to contact. Contact is an approximation that leads to these issues:

• Patchy stress results. For the internal gussets that are perpendicular to the outside plates, the real contact is along a line, but the contact elements in the analysis spread the load over an area. (This is shown well in the second post with 1 attached image.) With random node locations, the force distribution is somewhat random, and that leads to the patchy stress.
• For the splice plates where the two plates are in the same plane, the low stress right-along the joint occurs because the contact force is low at the nodes along the edge and higher at the next line of nodes. I would not have expected this, but I can duplicate it in the attached test model "flat plate.ipt". (Similar but slightly different issues occur when using solver contact and manual contact.)

Figure 2: Three flat plates with a tension force. The top half of the image shows the contact force. The bottom half of the image shows the stress.

• The joint on the left is defined using manual contact with the nodes at "1" (the Primary face) connected to the nodes at "2" (the Secondary edge; that is, Edge to Surface contact.) Because the contact force "1" is low at the edge and higher at the next line of nodes to the left (why?), the stress is low at the edge. Since the contact at "2" is only with the nodes on the edge, the contact force occurs at the edge and the stress is as expected.
• The joint on the right is defined using solver contact. For both sides of the contact "3" and "4", the contact force is low at the edge and higher at the next line of nodes away from the edge (why?). This results in a low stress right at the edge which is what you are seeing in your results.

My guess is the model is too complex to get continuous mesh to work. Have you tried continuous meshing? ("Mesh > Mesh Settings > Continuous Mesh") Continuous mesh matches the nodes between all the surface bodies and eliminates the need for the contact. That is, continuous meshing creates a perfect bond between the bodies instead of needing an imperfect bond created by contact.

That brings us back to my "first question for the Inventor modeling experts". The outside faces can be created by using a single solid instead of separate surface bodies. When defining the shell idealizations, you select the faces of the solid. See the attached example. All the shells created from the surface of the solid would be connected together without needing contact and without needing continuous meshing. The internal gussets would need to be surface bodies and therefore use contact or continuous meshing to connect them.

Let us know if you have any ideas or questions.

John

[kseminsky]

John, 

Thank you as always for your input. I have been playing around with some small scale tests, as you have, and finding that the BEST model is to node match (continuous mesh) all parts, thus eliminating the need for the contacts all together. Otherwise, stresses near the joints are inaccurate and hard to size welds from the results. It may be something I have read somewhere else that the contact elements are "infinite" stiffness.. (please verify?) Thus with infinite stiffness, no deflection, resulting in very low stresses at that location. Makes sense, but not good. FUTURE DEVELOPER IDEA! Add input values for contact element material properties???

So, on the modeling side of Inventor, I can use the thicken/offset command to create shells. It is a bit of work, but it seems to be effective. I would really like to know if there is a better way! Here was my work process. I made a simple model of 4 solid bodies (a single .ipt file), see below. 

Use the Thicken/Offset in Modify tab.

Turn on Surface Mode. Click face, Direction, and type half thickness.

For a test, I am going to make these two parts with Inventor Environment, and see if mixing with Nastran generated midsurfaces will work. Thought here is to node match in areas of concern where I need better results, then allow contact generator to take care of the rest. That would save me a lot of work.

Use the extend command in Surface tab to bring edge to adjacent plate:

Here is the two shells created in Inventor, leaving the other two as solids going into Nastran:

NOTE: I have found that prior to going to Nastran environment, you need to hide the solid bodies. Otherwise, the solids can not be turned off in Nastran (at least, I can’t figure out a way. If you turn off “CAD bodies”, you loose visibility of the shells too).

I was able to generate the remaining two plates using the midsurfaces command in Nastran. I then meshed and turned on the continuous meshing option. The edges of the two vertical plates node matched, which is great! So, it doesn't matter if the shell is modeled in Inventor or Nastran, the system recognizes the matched edge, and meshes properly. Good news here! Then, on purpose, I allowed the midsurfaces generator to leave a gap at the top plate to try a mix of contact elements and node matched idealizations. Here is the final mesh:

The results reflect what John has discovered in the gap area with contact elements. Low stress at the edge of the joint and poor stress gradient. The areas where there is node matching, the gradient is good. Notice I modeled 1/2" plate and 3/4" plate at the node match joint, and results look as expected. 

@John_Holtz Your help is very much appreciated. I look forward to learning where this goes from here. 

[John_Holtz]

Here are some answers to your questions and observations.

1. You do not want to use the stress results to size the welds when using contact. You want to use the contact forces and do a hand calculation to size the weld (or use the weld calculator in Inventor). Here is a video that describes the process. Predicting and Validating Welds with FEA in Autodesk Nastran In-CAD - YouTube. The one problem with this procedure is offset bonded contact with shells does not output the moment result; it only outputs the force result. I do not remember if Vince Adams describes how to handle that in the video.
2. Contact is not infinitely stiff. It is as stiff or weak as you make it by changing the Stiffness Factor value from 1 to x. (The solver calculates the default value based on the materials and element size. You scale that value by the Stiffness Factor.)
3. Your steps to convert a solid to a surface are similar to mine: How to convert a solid model to surfaces - Autodesk Community. As the saying goes, "great minds think alike". 🙂

John

[kseminsky]

Thank you for the reference info, I will need to take the time to watch that weld size video, seems very helpful for a lot of what we do. 

Can you elaborate on the stiffness of the contact elements? If what you say is true, and the solver determines a best suited stiffness, why then do we get the low stresses at joints and transitions? And, if we can adjust the factor, what does that really do? How can I control and expect that the contact elements are acting as the adjacent materials? I will play around with this a bit to see how the factor affects the results. 

I have been working on converting my solid model to shells manually, and the process is working well. It just takes time. 

[John_Holtz]

The low stress is not related to the stiffness of the contact. The low stress is related to where the contact is created and which nodes are connected to which nodes. The solver does not provide enough control to let you change the where part of the contact (other than changing the maximum activation distance which is not related to this issue).

I have updated the previous image to better show how the contact is created in my test model.

1. I put a gap between the three sections of shells (the bottom row of the figure) to better illustrate that the shells are not physically connected together. (Whether the gap is 0 or some value does not change the description.)
2. The arrows show the contact forces; that is, where the contact elements are transferring the load between the sections.
3. In the elements identified as "F", the elements are transmitting the full applied load. Therefore, the stress is as expected = F/Area.
4. In the elements identified as "T", the contact force is distributed over the element. The stress in the elements is lower than the average stress F/Area.
5. In the elements identified as "N", there is either no contact force in the elements (such as in shell 1), or a very low contact force (such as the connection between shell 2 and 3). The stress is 0 in these elements. Why the contact is skipping the nodes closest to the connection is unknown.

Keep in mind that contact is placing springs between the nodes on one side of the contact to the elements on the opposite side of the contact. Depending on the materials, the default contact could be too stiff or too weak. (Too stiff can cause convergence difficulty or restrict the elements from expanding/contracting. Too weak can allow the parts to separate or penetrate.) The "Stiffness Factor" that you enter on the contact dialog multiplies the default stiffness. By changing the stiffness, you can compensate for the types of problem when the contact is too stiff or too weak.

Hope this helps.

John