ERROR#4965
hi，I have been doing a simple simulation recently, the material is nonlinear, so the loadstep is set to nonlinear quasi-static analysis, but there is no error when applying a uniform load of 50KN, and there is a mistake when changing to 100KN uniform load.
*** ERROR # 4965 ***
Maximum number of time increment cutbacks reached,
analysis aborted.
*** Nonlinear solution failed to converge for Subcase 1 ***
I don't know how to solve it，could you give some advices？
here is .out file. thank you.
Answers
-
Please try by referring below post last comment. If possible migrate to newer version 2018 . OptiStruct 2017.2 support large displacement for composites.
https://community.altair.com/community?id=community_question&sys_id=d376083a1b2bd0908017dc61ec4bcbff0 -
Your model failed to converge beyond 41% of total load- possibly due to buckling.
Models with geometrical (large displacements, rotations, buckling), material (plasticity and rupture) and contact (sliding, friction, open/close) nonlinearity are more efficiently solved with explicit method. If nonlinearities are severe (crash and drop tests) then explicit is the ONLY option (also including inertial effects).
0 -
Altair Forum User said:
Please try by referring below post last comment. If possible migrate to newer version 2018 . OptiStruct 2017.2 support large displacement for composites.
I try to increase the NCUTS as 10.even 100.It still not work。
0 -
This question needs to be solved urgently. Can you give some suggestions? Thank you
0 -
Did you try this in latest version?If possible share the .fem file which you are running at your end.
0 -
Altair Forum User said:
Did you try this in latest version?If possible share the .fem file which you are running at your end.
I con't find the latest version，and try many times，but I don't solve it，here is my .fem file
0 -
I took a quick look in to your model and felt the load magnitude which you are applying is quite high. I see you are applying magnitude of 1000N on each node which would be overall as 20100N.If you want to apply 1000N on that face then simply count the no of node falls on that region and divide it by the force magnitude.201/1000 =.201
Please update the load with .201 N on each node and run again with ncuts as 5 (default)
0 -
I am sorry that 1000KN is not use，I forget to delete it，the useful load is supress load collector，overall 20000N，just one compress case.
here is update .fem file
0 -
Either convert (tools>convert>optistruct>to Radioss) and solve in Radioss or use Nonlinear direct transient analysis in Optistruct.
Check these tutorials and examples:
OS-T: 1310 Direct Transient Dynamic Analysis of a Bracket
OS-E: 0200 Beam Bending
OS-E: 0205 Car Bumper Impact
OptiStruct Nonlinear Learning Center
Also check the attached chapter from free eBook: Introduction to Nonlinear Finite Element Analysis using OptiStruct
The latest model you shared still fails to converge beyond 35%. One of the reasons is because high concentrated loads are applied on only two nodes. This is unrealistic (applying 1 tonne of force on a single node, similar to introducing the load through a needle leading to high-stress concentrations) and also causes numerical difficulties. A more sensible approach would be to apply the same force as pressure load or distribute it over more nodes. However, the computation will still probably diverge in case of buckling instability.
0 -
Attached are Radioss model file and result. The load is linearly ramped up over 0.3 seconds.
Surprisingly the pillar did not buckle, but the stresses are huge (almost 4GPa) so it would fail across the top and at the base.
The image shows elements exceeding 1000MPa in red.
<?xml version="1.0" encoding="UTF-8"?>
0 -
I tried Non—linear transient analysis，but it runs very slowly，After running for several hours, there is still no result.
I don't know where is wrong.here is .fem file，.
could you check and modify it？thank you
by the way，the model you provide seems to Incomplete，
0 -
As mentioned before, highly nonlinear models can be solved only with the explicit method.
The Radioss model was updated to include material nonlinearity. This model buckled approximately at 40% loading near the top and again at 70% near the base (see attached animation and graph). An implicit method would fail to converge at those points.
<?xml version="1.0" encoding="UTF-8"?>
Attached is the revised Radioss model and explicit dynamic Optistruct model (it runs Radioss in the background).
0
