Grid point identified in error not found in model

[kseminsky]

I have a rather large and complex model under static structural analysis, Inventor 2021, Nastran 15.0.0.187. I have been troubleshooting an E5000 error. I enforced the sparce direct solver (VSS), which then provided a gridpoint (206521 in my model) where the singularity is occurring. When I search for this grid point using the "highlight" command, I get the error that the grid point does not exist in the model and has been removed, see image attached. 

Really confused here? I've made many adjustments to my model constraints and end releases on my line elements, and the E5000 at this same grid point occurs. This latest attempt I removed all end releases, and still get the error. Side note, the solid elements in my model are created from a single "monolithic" part (no surface contacts, all nodes match) and the line elements are connected to features using rigid elements. I feel certain I do not have any parts "flying" away. All intersecting line elements are also node matched (sketch lines terminate and connect at intersections). But I must be missing something...

This model takes over 2 hours to generate the nastran file (before the "Nastran Output" window is even started)... Making changes and re-trying is extremely time consuming, so any thoughts are greatly appreciated! Thank you. 

[John_Holtz]

Hi @kseminsky 

I cannot imagine why a model with 200000 nodes takes 2 hours to create the Nastran file. Something else (besides the E5000) is wrong and is creating a lot of entries (a lot of lines) in the Nastran file. For example,

• Are there forces applied to faces that have a lot of elements? That is one reason that I know if that requires a long time to created the Nastran file. (I see some forces applied to nodes, but nothing obvious applied to faces/surfaces.)
• Do you have contact defined? If so, did you use Auto, Manual, and/or Solver? How many contact pairs are listed in the browser?
• (edit) Is the model saved on a network drive? Network communication could be slow.

The command to highlight nodes only shows node numbers created by the mesh. It does not show the node numbers created by connectors. My guess is the node number 206521 is the center point of a rigid body connector or at the ends of a bolt connector. Here's another way to find the node 206521:

1. Edit the Nastran file using Notepad.
2. Locate GRID 206521.
3. Write down the coordinates. See How to get node coordinates in Nastran In-CAD or Inventor Nastran. (See the Note below regarding the spreadsheet that is attached to the article.)
4. Go into the modeling workspace in Inventor. (Exit Inventor Nastran if necessary).
5. Use "Assemble > Work Features > UCS" or "3D Model > Work Features > UCS" and create a mini-axis on the model at the coordinates from step 3. This puts a nice mini-axis at the problem area. Once you know the location, you can determine why the model is unstable in the X direction ("Component 1" given in the error message).

Note that the spreadsheet attached to the article will download as a zip file. It is not a zip file. Change the extension to .xlsm if you want to use the spreadsheet. Alternatively, use FNO Reader instead of the spreadsheet. I will try to get time to update that article today.

[kseminsky]

@John_Holtz 

Thank you for the quick reply. I did have quite a few forces over many surfaces (mostly weights of equipment that are bolted to the structure). I re-applied them either through rigids or edges/nodes on the solids rather than surfaces. The file now writes in about 15 minutes, huge improvement!! Thank you for that! Regarding contacts, there are none in this model. My solids are generated from a single monolithic part. Just to confirm that everything is bonded, I did run the "auto" contact generator, and no contacts were created. I am running this model on my local solid state hard drive. 

I pulled the grid location from the .nas file: 

It was a little tricky determining what was X, Y, Z, and I am still not 100%, please verify I interpreted these values correctly. At this location in my model, there are no rigid connectors, in fact, it doesn't even land on a node:

I understand that if a random node in a solid structure is flagged as a singularity, it could mean the entire body is not supported in space. considering that, I re-ran the model with a true fixed constraint to ensure that the entire body is constrained. Got same error, but different grid number and now component 3. It's location is very near the first grid.. 

Thank you again for your expertise, I very greatly appreciate it!! Hoping you may still have some thoughts? 

[John_Holtz]

Hi,

You interpreted the coordinate correctly but mis-typed the Z coordinate when creating the UCS. So the UCS is off by 0.4" in the Z direction. 🙄

It may just be the view angle in your image, but it looks like the mesh at the UCS does not match with the item in the background. Maybe there is a gap between the parts and they are not supposed to match, but it made me think of something else.

Does the model contain multiple bodies? Inventor can create separate bodies in a single part file. Nastran treats them as separate (the mesh is not continuous from one piece to another), and the "Contacts > Auto" command does not detect that there are parts touching -- because there are no parts touching. (There are bodies touching, but Nastran is not programmed to detect separate bodies).

If you have separate bodies, the top of the tree in the Inventor Model tab will show "Solid Bodies (15)" or how ever many there are. In this case, your options are to combine all of the bodies into one body, or manually define the contact between the bodies. (You can define one "Contacts > Solver" and use a "Maximum Activation Distance" less than half the mesh size to bond everything in the analysis to everything else.)

Note that you can also change the analysis type to "Normal Modes" and calculate the first several natural frequencies. Pieces that are not constrained and give the E5000 (or E5001, E5004) messages in a static analysis will have a rigid body mode in the modal analysis. The frequency will be near 0, and the displacement will show which piece is free to move.

[kseminsky]

Thank you for the additional thoughts. The mesh is matching through all the features, and I did confirm that I have only the one solid. I did use the combine command before bringing the part into FEA to "seal" all the surfaces as one part. 

I ran the normal modes analysis, set it up to solve for the first 5 frequencies up to 100hz. Here are the results from that. I am not seeing any parts separating, all looks in order:

Any other thoughts? I am really stumped on this... I might just try to re-build this analysis entirely, maybe there is a glitch? 

[John_Holtz · Accepted solution]

Hi,

I'm stumped too! If you can provide the model (zip the assembly and part files, .iam and .ipt), then someone will take a look.

Technically, there are three different things that can cause the E5000 errors:

1. A piece of the model is not constrained so it is free to translate in X, Y, or Z, or is free to rotate about X, Y, or Z.
2. The material properties are wrong, or the largest elastic modulus in the model divided by the smallest elastic modulus is so large that the analysis "thinks" the weak material is free to move due to insufficient strength. (Generally, a range of 1000 to 1 is large enough to simulate a stiff versus weak material.)
3. The mesh contains distorted elements. You can right-click on "Mesh Model" in the model tree and choose "Check Quality for Mesh > Jacobian < 0.1" and see if there are any elements with really small (or negative) jacobians.

However, I do not remember a situation where the stress analysis encounters the E5000 error but the modal analysis runs without showing any problem. The only situation is when the linear stress analysis includes separation contact. The Normal Modes analysis replaces separation contact with bonded contact, so a part that is under-constrained in the linear analysis can become bonded in the Normal Modes analysis and appear to be okay.

[kseminsky]

@John_Holtz 

I checked the points you suggested. Since the modal looked good, I am with the assumption that nothing is free to translate. I made a few runs applying additional constraints, just to see if the model would make it to a solution. Got a new grid point with singularity (still E5000 error). Still on the solid mesh in a random location:

Material properties seem to be applied correctly through the idealizations. All my materials are steel, with the exception of some short "strong but light" elements to simulate rigid connector elements with the ability to release end nodes for rotations. Here are the properties I applied for those. Based on what you said, maybe I need to lower the elastic modulus here? I've used similar properties before without issues:

Lastly, the jacobian error. The nastran file indicates tetrahedron skew angle errors (which seems to be typical for these larger analyses) for a handful of elements. I ran the mesh quality check with jacobian <.1, here is what it generated:

 I am going to refine the mesh a bit more, and also lower that elastic modulus in the "rigid" elements, and see if any of that helps. Will post back. If this next refinement doesn't work, I'll see if I can share a model file for further diagnostics. Thanks again for your help and suggestions!

[kseminsky]

UPDATE: With the changes mentioned, I was able to get a solution!! Very greatly appreciate the support @John_Holtz  Thank you!!! 

I refined the mesh, which now contains just over 300,000 elements, only about .26% having jacobian below .1. Also, I corrected the Rigid material properties: