I am doing a contact analysis between two plates (sol 601- 106), the modelling I did was similar to a video I found on Youtube (https://www.youtube.com/watch?v=D6QaR9nB-RA&t=1s). It is a very simple model, but when I try to run to solver it does not run. I got a fatal error message, see picture. Does someone have an idea what the problem could be? (error in model, setting in NX,...) ?
thanks in advance!
Solved! Go to Solution.
Post here .dat and .f06 files. With your description I can say that you doing something wrong) Note that error desctiption in sol 601 placed somewhere in the middle of .f06 file, not after line "USER FATAL MESSAGE ", so you must check all file (as you see fatal message indicates only error in sol601 without any additional descriptions and codes of error).
Here is small part of your model.
The error message in your F06 file is:
*** ADVANCED NONLINEAR ANALYSIS *** *** FATAL ERROR: INPUT FILE advnlin.op2 NOT FOUND. *** PLEASE MAKE SURE THE NASTRAN INPUT FILE CONTAINS THE FOLLOWING LINE ASSIGN OUTPUT2='advnlin.op2',UNIT=21 *** AT THE BEGINNING OF THE FILE. *** ISHELL PROGRAM 'NXNA' COMPLETED *** ^^^ USER FATAL MESSAGE ^^^ ERROR IN ADVANCED NONLINEAR MODULE 0 ^^^SOL601 FAILED
but this line is exist in your model. It may be problems with Nastran inatalation.
As for your model:
1) the model is non constrained well - you also must constrain big plate, also in every node, where you have thanslational load you must constrain node in the direction of load, in nastran enforced motions is more like constraints that applied like loads.
2) in nonlinear analisys you select only one time step to solve model, a good assumption for model is 50-100 timesteps,then you can reduce timestep until your solution remain stable. Also use automatic time stepping to gen better convergece. And with your setting with one timestep with time interval of 1 sec you calculate only one second, but function load goes to 10 second.
3) not critical - meshing plate with one row of tetrahedral elements without midside nodes is the worstest case, to get good results mesh 3-5 elements pers thickness with hexa elements or use plate element, you can also use tetra elements with midside nodes instead of hexa, but you get aproximately 8 times more elements on the same detail with same mesh size.
Model contact problems on the simple models like two bricks with 100 elements or less, and when you be familiar with all settings and get reasonable results - proceed to real models.
Thank you for the response. For the error 'INPUT FILE advnlin.op2 NOT FOUND.' I just need to reinstall to fix this? Or if I adapt the model I will be able to see the results?
Try to run my model. Import it to NX or run through bat-file and if all calculated properly, then thiss error in not cause but consequence of other errors like I mentioned before. Note that some setting can be lost during translation from .dat file to NX. You cal directly execute .dat file witt Nastran solver - run file nastran64L.exe and select my dat file.