Jump to content
Amasker

ERROR#4965

Recommended Posts

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.

bend-100KN_LGDISP.out

Share this post


Link to post
Share on other sites

@Amasker

 

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).

 

Share this post


Link to post
Share on other sites
11 hours ago, Rahul R said:

Please try by referring below post last comment. If possible migrate to newer version 2018 . OptiStruct 2017.2 support large displacement for composites.

 

 

Thanks,@Rahul R

 

I try to increase the NCUTS as 10.even 100.It still not work。

Share this post


Link to post
Share on other sites

Thanks ,@Ivan

 

How to choose the loadsteps with explicit method,I have never used this method,only related to material nonlinearity,

 

could you give some cases or tutorials?thanks in advance.

Share this post


Link to post
Share on other sites
On 3/12/2019 at 7:34 PM, Rahul R said:

Did you try this in latest version?If possible share the .fem file which you are running at your end.

 

@Rahul R

I con't find the latest version,and try many times,but I don't solve it,here is my .fem file

 

Share this post


Link to post
Share on other sites

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)

Share this post


Link to post
Share on other sites

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

 

Share this post


Link to post
Share on other sites

@Amasker

 

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

41adadc6f1d0fee92622775413b90791a0e7a377.jpg?image_play_button_size=2x&image_crop_resized=960x614&image_play_button=1&image_play_button_color=54bbffe0

OptiStruct Nonlinear Learning Center

Also check the attached chapter from free eBook: Introduction to Nonlinear Finite Element Analysis using OptiStruct

Nonlinear Direct Transient Analysis.pdf

 

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.

Share this post


Link to post
Share on other sites

Attached are Radioss model file and result. The load is linearly ramped up over 0.3 seconds.

amasker_radioss1.hm

amasker_radioss1.h3d

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.

pillar.jpg

Share this post


Link to post
Share on other sites

Thank you @Ivan

 

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,original_steel_supress.fem.

 

could you check and modify it?thank you

 

by the way,the model you provide amasker_radioss1.hm seems to Incomplete,

Share this post


Link to post
Share on other sites

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. 

pillar_buckling.gif

Attached is the revised Radioss model and explicit dynamic Optistruct model (it runs Radioss in the background). 

 

amasker_expdyn.hm

amasker_radioss_0000.rad

amasker_expdyn.fem

Share this post


Link to post
Share on other sites

Join the conversation

You can post now and register later. If you have an account, sign in now to post with your account.

Guest
You are posting as a guest. If you have an account, please sign in.
Reply to this topic...

×   Pasted as rich text.   Paste as plain text instead

  Only 75 emoji are allowed.

×   Your link has been automatically embedded.   Display as a link instead

×   Your previous content has been restored.   Clear editor

×   You cannot paste images directly. Upload or insert images from URL.


×
×
  • Create New...