Hi everyone,
I'm encountering an issue in Autodesk Inventor Nastran with a simple model I've intentionally under-constrained. The model is a tube that is only constrained to allow rotations axis at one end. However, when I run the analysis, the solver completes without errors and produces reaction moments in the results.
This is confusing, as I deliberately left the rotations unconstrained to observe the effects. I expected the solver to either fail due to insufficient constraints or show free rotation without any reaction moments.
To clarify:
I've attached a picture of the model and the model file itself for reference.
Has anyone encountered a similar issue? Could this be a result of how the solver handles under-constrained systems? Any suggestions or insights would be greatly appreciated!
Interestingly, when I calculate the same model directly in Inventor (without Nastran), the solver behaves as expected and returns an error indicating insufficient constraints. This makes me wonder if there's something specific to how Inventor Nastran handles under-constrained systems.
Thanks in advance!
Hi @WernerBeek
The image and model did not get attached. You may need to log into the forum and upload them manually to the post.
My guess is you are using solid elements. Solid elements do not calculate the rotations, so freeing the rotation constraints is doing nothing. That is, a constraint of TxTyTzRxRyRz on a face of a solid is identical to TxTyTz.
For a solid part to "rotate", the nodes need to translate in the hoop direction. Chances are you have that translation direction fixed (TxTyTz) so you are actually preventing the tube from rotating. What you could do is use a rigid connector on the end of the tube and put the constraint (with rotation not checked) at the center point of the rigid connector.
You are correct that Nastran can add some artificial constraints to solve an under-constrained model. It does that because the parameter AUTOSPC is set to on. (If you have contact in the model and are using parabolic elements, you need to have AUTOSPC set to on.) If you change the Parameter to Off and the analysis runs, then the model is not under-constrained. If the analysis ends with E5000, E5001, or E5004 error, then the model is under-constrained.
Hope this helps.
John
Hi John,
Thank you again for your detailed explanation and suggestions!
I tried implementing the rigid connector approach as you described. I added a rigid connector at the end of the tube and applied the constraint (with rotation unchecked) to the center point of the connector. However, after running the analysis, I still see reaction moments being calculated in the results, which seems unexpected.
Regarding the AUTOSPC parameter, I understand its purpose now, but I’m not sure where I can find it in Autodesk Inventor Nastran. Could you guide me on how to locate and modify this setting? I’d like to test the model with AUTOSPC turned off to confirm whether the model is truly under-constrained or not.
I’ve also uploaded the model file and an image of the setup for further reference. Hopefully, they can provide more context for what might be happening.
Thanks again for your assistance—it’s greatly appreciated!
Best regards,
Werner
Sorry, I forgot to mention that Parameters are set using the Parameter branch at the end of the model tree (actually, the second branch from the bottom).
I will look at the model later, but my guess is face 32 is fixed in X, Y and Z translation, so the reaction forces are preventing rotation. Since moment = distance*force, there is plenty of "moment" reaction about the origin due to the reaction forces. See Tip 49 in the PDF document attached to my forum post Suggested Reading - Tips and Tricks on the Inventor Nastran forum.
John
Hi John,
Thank you for your feedback and the reference to Tip 49 in the PDF.
I’ve made the adjustments you suggested:
Despite these changes, Nastran is still able to solve the model and produce results, including reaction moments. This is puzzling, as I expected it to fail or reflect the under-constrained nature of the model.
Best regards,
Werner
Hi Werner,
Is the constraint located at the origin? If not, the distance from the origin to the constraint times the reaction force creates a moment about the origin.
Normally, you want to get the node number where the constraint is applied, and enter that node number in the dialog instead of using the origin. It is best to open the Nastran file with Notepad (or any text editor) and search for RBE2. The description right above the hit will tell you which connector you found. The third column gives the node number at the center of the connector. (Or search for SPC1. The fourth column gives the node number where the constraint is applied.)
John
I understand that all constraints are being referenced using the origin as the reference point. This raises a question for me: what is the logic behind this? Shouldn’t the reaction forces and moments ideally be calculated relative to the local coordinate system of the applied constraint?
Having to manually identify the central point seems counterintuitive. If I can locate the central point manually by examining the Nastran file, wouldn’t it make sense for Nastran itself to provide this information directly in the output?
It feels like this could simplify the process and reduce the likelihood of errors. Is there a specific reason Nastran doesn't handle this automatically, or is there an option to make it output reactions relative to the applied constraint's coordinate system?
Sorry, I forgot to reply to your question of "Is there a specific reason Nastran doesn't handle this automatically". The answer is there is no good reason why Inventor does not do it. Maybe the developers will work on it sometime in the future.
John
Can't find what you're looking for? Ask the community or share your knowledge.