2D Crack Growth with Inclusion - Tutorial not working with 6.12

[thestock]

Hello all, thank you in advance for taking a look at this.

I'm a new ME grad student trying to learn Abaqus and I'm having trouble with a crack growth tutorial.

Link Tutorial

Link CAE file

It may work for v6.9 but it's not working for v6.12.

I downloaded the .cae file and run into the exact same issue as when I tried going through it step by step.

When running the job submit, I always get, "Error in job IncCrack: Too many attempts made for this increment." "Aborted due to errors."

Any ideas?

Thanks again, this is all VERY new to me although I had some experiance with ANSYS a few years ago.

Daniel

 

[burningDiesel]

Most of the time, abaqus updates to the solver and settings cause a better convergence of the problem. Apparently, in your case it's the opposite.

To make it work you can:
1. decrease your mesh size (this will probably help) or use normal elements instead of reduced elements.
2. decrease the maximum time increment: everything goes fine until the thing starts cracking, and the solver needs to decrease the incrementation size, but it reaches the default 5 step backs before being able to solve the increment, i.e. "Too many attempts made for this increment".
2b. Change the default incrementation settings, I changed the default 0.25 step back to a 0.1 one, so you can calculate fast in the beginning, and cut back fast too. This is not advised.

So changes to make it work are:

*Element, type=CPS4
*Static
0.05, 1., 1e-08, 0.05
*Controls, reset
*Controls, parameters=time incrementation
, , , , , , , 8, , ,
0.1, , , , , , ,

Also, no student posting here, ask your supervisor next time.

 

[thestock]

Thank you for taking the time to look at that file and the thorough response.

I didn't realize grad students weren't allowed but I won't post anymore threads.

My supervisor is trying to learn this software as well so I'm not able to get any help there.

Do you have a suggestion where I should (or can) get information and help from time to time?

Thanks,

Daniel

 

[burningDiesel]

I don't really know, there is a linkedin group, and a yahoo usergroup, I don't know the policy on student posting.
But if you ask good questions (and not homework assignments), maybe you can get away with it here

 

[thestock]

Oh! I understand what you mean now. No, this is not for a class. This is (most likely) what I'll be basing my thesis on.

In that case I'll pick your brain some more if you don't mind.

I spent a couple hours trying to implement your suggestions:
[ul]
[li] 1. Decrease mesh size - I decreased all the way to only 5 nodes per edge and still had the same error.[/li]
[li]2. Decrease max time increment - If that's the increment under Step - Loading, I changed to 0.05, 1, 1e-08, 0.05 but still had the same error.
[li] 2b. Increment setting - I wasn't sure how to change this but you didn't recommend it anyway.[/li]
[/ul]

This looks like part of you INP file, right?

*Element, type=CPS4
*Static
0.05, 1., 1e-08, 0.05
*Controls, reset
*Controls, parameters=time incrementation
, , , , , , , 8, , ,
0.1, , , , , , ,

I tried changing the INP file but realized when I hit submit it was just overriding it.
I changed the INP file to match what you posted and then imported into a new file. Running this still had the same error.

The only way I could get it to run without errors was to decrease Load (pressure) from -700 to -300 but that was not enough to actually create any deformation.

 

[thestock]

 

[burningDiesel]

I got the inp file on another pc, I'll upload it tomorrow if I don't forget.

What I did was 1. change the element type from reduced to normal:
Refining the mesh probably has the same effect.
*Element, type=CPS4

2. Decreased the minimum allowed time increment:
*Static
0.05, 1., 1e-08, 0.05

3. And set the default cutback to a factor 0.1 , and the maximum number of allowed cutbacks to 8:

*Controls, reset
*Controls, parameters=time incrementation
, , , , , , , 8, , ,
0.1, , , , , , ,

You can check documentation for these keywords to see the way to do this in CAE.
You can run .inp 's by doing
abaqus analysis job = jobname.inp
in command line

 

[loki3000]

http://www.matthewpais.com/contact

contact him and maybe persuade him to also update the page (or at least post what he told you here for future ref). he works for dassault simulia anyway so it couldn't hurt...

 

[femfunm]

@sdebock What is a thumb rule in order to make modifications to cutback factor and to the maximum number of allowed cutbacks as you did in the certain problem and how we can ensure the onset of the crack?

 

[burningDiesel]

Normally the default does a good enough job. Changing the cutback factor and number of allowed cutbacks doesn't have a clear downside (apart from poorer performance). If you need to cut way way waaay back there probably is something wrong with your simulation.
Messing with tolerance values can have serious consequences on the result, so watch out with that.

For the second part of your question, in this example the crack is initiated, and growth depends on the material (damage) properties and loading.

 

[mar2805]

Could ABAQUA be used to model cracking of reinforced concrete elements?