Result File is in wrong format - NX 7.5
Result File is in wrong format - NX 7.5
(OP)
I'm trying to do a simple FEA static load on a lower control arm in NX 7.5, and everything appears to be working, except I cannot do any post processing b/c it says the "Result File is in wrong format." The .f06 file has no fatal errors listed, and I've tried the param, bailout, -1 procedure without any luck.
The data appears to be writing to a .dat file. Failing the ability to post-process in NX, is there another processor that I could run the .dat through and still get results and animations?
The data appears to be writing to a .dat file. Failing the ability to post-process in NX, is there another processor that I could run the .dat through and still get results and animations?





RE: Result File is in wrong format - NX 7.5
Regards,
Mark
Mark Lamping
CAE Technical Consultant
Siemens PLM Software
RE: Result File is in wrong format - NX 7.5
RE: Result File is in wrong format - NX 7.5
There is one other possibility. Does the model have any constraint (RBE2) elements in it. Searching a Siemens PLM internal mailing list led me to a reported post processing limitation that's been extended/removed. The limitation was related to a model that contained an RBE2 element with 33484 nodes. That's not a typo... 33484 nodes for one element! NX 7.5.2 and prior versions support models with single elements defined by up to 32767 nodes. NX 7.5.3 and higher versions support single elements defined with up to 2 GB nodes. So this limitation has been virtually removed.
Regards,
Mark
Mark Lamping
CAE Technical Consultant
Siemens PLM Software
RE: Result File is in wrong format - NX 7.5
USER FATAL MESSAGE 9137 (SEKRRS)
RUN TERMINATED DUE TO EXCESSIVE PIVOT RATIOS IN MATRIX KLL
That led me to the param bailout -1, which removed the fatal error but still gives me the error on the output file. I see no other warning or errors in the .f06 file.
There shouldn't be any contraint elements, though I do see that I have 49,673 nodes now from 36,503 elements. I'm constraining it by a fixed constraint on the inside face of the bushing mount, could that be causing a problem?
Thanks for the help
RE: Result File is in wrong format - NX 7.5
1. Open the SIM file
2. Select the SIM file in the Simulation Navigator
3. MB3 Simulation Summary
This will print out a summary of nodes/elements, boundary conditions and such. How many solid/sheet bodies are meshed? This could probably be solved with a quick view of the model. Doing it here is more challenging. You may want to consider opening a call with GTAC so that you could show the support AE the model and get some quick advice.
Regards,
Mark
Mark Lamping
CAE Technical Consultant
Siemens PLM Software
RE: Result File is in wrong format - NX 7.5
RE: Result File is in wrong format - NX 7.5
How are you assuring that the shell elements are connected? I suspect that there are regions of your shells that are completely disconnected from one another. Further, those elements have no path to the constraints you defined, so they are free to move rigidly (a linear statics no-no). If the CAD geometry is manifold, then you can sew the sheet bodies together to form (for example) 1 body from 2 bodies. Non-manifold connections (such as two sheet bodies forming a T intersection) can be connected in the FEM polygon geometry using the Stitch Edge command. Sew in CAD and Stitch Edge in CAE polygon geometry will produce shell-shell connections (i.e. shells that share nodes/edges) and a contiguous mesh.
Your control arm should be one contiguous mesh but I suspect it isn't. At this point you can check the shell mesh for element free edges. In the FEM or SIM select the Finite Element Model Check command (green check mark icon or Analysis, Finite Element Model Check from the menus) and set the dialog to Element Outlines. Apply the dialog and NX will highlight all of the shell element free edges. These are edges that don't connect to other shell elements. There are likely more free edges in your model than there should be since your input geometry is unstitched.
Another way to view the disconnected shell element regions is by performing a normal modes analysis. Every disconnected region will produce 6 rigid body modes. If you have 3 disconnected regions, you will get 18 rigid body modes.
If I'm correct here, I suggest you review the NX online help for the Modeling Sew command and Advanced Simulation Stitch Edge command.
Regards,
Mark
Mark Lamping
CAE Technical Consultant
Siemens PLM Software
RE: Result File is in wrong format - NX 7.5
RE: Result File is in wrong format - NX 7.5
I've had similar problems (usually solved by deleting everything and starting again) in the past, which is why I ask.
RE: Result File is in wrong format - NX 7.5
Regards,
Mark
Mark Lamping
CAE Technical Consultant
Siemens PLM Software