topic Troubleshooting Grid Point Singularity E5010 in Inventor Nastran Forum

Troubleshooting Grid Point Singularity E5010

kseminsky — Mon, 11 Mar 2019 13:41:30 GMT

I have a model containing line, shells, and solids. During the solution process of each subcase, I am getting an E5010 warning. There is a slight discrepancy in the deflected shape (applying a test symmetric load on a symmetric model, and getting non-symmetric deflection). I'd like to pinpoint the grid that is causing the issue so I can further review and either dismiss the warning, or make a correction in the model. The on-line help suggests to "Check the Grid Point Singularity Table in the Model Results Output File for degrees of freedom that should not be auto-constrained".

Where/How do I review the "Model Results Output File"? A detailed step-by-step to locate the exact grid/element that is causing the warning would be very greatly appreciated. Thank you!!

Re: Troubleshooting Grid Point Singularity E5010

g.ceruti — Mon, 11 Mar 2019 14:33:23 GMT

Hi @kseminsky ,

you can find the Model Results Output File (the *.out file) in the subfolder "yourfilename\InCAD\FEA\" where your *.ipt or *.iam are file is opened.

The *.out file is a text file, so you can open it with each text editor like notepad.

The print out of Grid Point Singularity Table is always active, unless you turn it off using the following parameter: PARAM,PRGPST, OFF.

Re: Troubleshooting Grid Point Singularity E5010

kseminsky — Mon, 11 Mar 2019 17:33:29 GMT

Great, thank you for the quick response!

I dove into the file, and found the grid point singularity table. I am not sure how I am able to identify which grid points were auto-constrained? I attached a screen image of the last page where the warning occurs for "subcase 1". Note that this occurs for all 3 of my subcases.

Much appreciate the help. Thanks!

Re: Troubleshooting Grid Point Singularity E5010

g.ceruti — Tue, 12 Mar 2019 07:41:29 GMT

I suppose you are using a 3d tetra mesh.

When you use 3d Tetra solid elements, since they don't have any stiffness associated to the rotational degree of freedoms (d.o.f. 4,5, & 6), you always find 3 lines for each node (like for 426101 or 426107 in your table).

I think that Nastran applies the suitable constraints to all the d.o.f. listed in the singularity table, if the AUTOSPC paramenter is set to On.

(http://help.autodesk.com/view/NSTRN/2019/ENU/?guid=GUID-E9B2A368-AE44-466E-B867-4E8DBA91379C)

However you can verify it, using the SPCGEN parameter set to ON, which enables the printout of the auto applied constraints.

(http://help.autodesk.com/view/NSTRN/2019/ENU/?guid=GUID-A2E6085D-CC4C-4702-8FB5-9EEAF72183FF)

I think that, if the singularities listed in the "grid point singularity table" are only related to d.o.f. 4,5 & 6, it should not be the cause of your un-symmetric response.