Removal of parts during analysis

[geo2006]

Hi everybody,

is it possible to "remove" a part during a simple 2D analysis using Abaqus/CAE? Accordingly to Analysis User's Manual, sec. 11.2.1, it can be made with the input

*MODEL CHANGE, TYPE=ELEMENT, REMOVE

but I'm using CAE. I'm trying to model the effects of a stepped excavation and need to take off portions of soil.

Thanks in advance.

 

[corus]

If you can't do it in CAE then use the Edit Keywords option and add in the lines you want to the input file, or just simply create the .inp file, exit CAE, and edit it with Notepad. There are some things that CAE can't do and you have to manually edit the file.

corus

 

[geo2006]

Thanks Corus, I'm just learning to use Abaqus seriously and I'm no yet very familiar with the input of data in text form (have to learn now!).

Just 2 more questions: I opened the inp file created with CAE. But where do I have to insert the new line? And with this new file can I continue using CAE?

Thank you very much.

 

[corus]

*Model change is in the Step section of the data. If you edit the .inp file within CAE using edit keywords then your edits will remain even if you alter the model soem tiem later. If you edit the .inp file in Notepad then the .inp file will be over written the next time you use CAE and create the input file. If you do use Notepad then it's best to save your original .inp file as something else and then use Winmerge to compare your old .inp file with the new one you might have created. That'll show you the differencse between the files and you can easily copy your edits from one file to the other.

corus

 

[conorjameswalsh]

hi there
I am having a similar problem. I too want to remove elementsbut want to do it to elements whos strain exceeds a set value.

Do you know how I can do this

Thanks

Conor

 

[geo2006]

Hi,

again, thanks Corus for your help. As I said, I'm just learning Abaqus, so sometimes little tips make the difference between solving a problem or giving up. I now have my model working fine.

To Conor: sorry, I can't help in your problem.

Regards
Fdo.

 

[Yoman228]

Conor

That a very intresting question, If you find out the answer. pls post here as I am quite keen to know how to slove it. Wonder any subroute will do the job

 

[geo2006]

just wonder...what if you define a material (using its stress-strain curve) in such way that exceeded some predefined strain its resistence drops near 0?.It would behave like removing it in some way. I'm wrong?

Regards.

 

[RGX124]

Hi Geo,

You can use cohesive elements for that purpose. There are well implemented in CAE since V6.6. Another way is to define a user element (UEL) with the wanted behaviour.

R.

 

[bassmanjax]

There's an even easier way to remove elements at a sepcified strain. Take a look at *DAMAGE INITIATION & *DAMAGE EVOLUTION.

Regards

Martin Stokes CEng MIMechE

 

[xerf]

Setting the material stiffness to zero may lead to convergence problems and mesh size dependency.