internal surfaces - perforation problem 2

[trickstersson]

Hello everyone!

I am modeling impact problem in Abaqus 6.12-1 (CAE). Rigid projectile with known initial velocity should perforate aluminium wall (Johnson-Cook damage model with damage evolution, so elements are deleted when the material fail).

Because surface elements fail and are deleted, INTERIOR elements will be exposed to contact. Manuals that i found on internet says that INTERNAL SURFACES must be created, modifying input file:

*SURFACE, TYPE=ELEMENT, NAME=ERODE
PLATE,
PLATE, INTERNAL

(where ERODE is exterior surface and PLATE is element set of perforated part)

The problem is because i can not add lines under *SURFACE in input file (i modify input file with keyword editor).

Any suggestions how to solve the problem or is there any other way to create INTERNAL SURFACES?

 

[trickstersson]

Hi!

I am afraid that I do not understand exactly what is your problem. As I understand your post, you are not sure where to put surface definitions in .inp file. If you are not sure where to put surface definitions in .inp file than try both: (1) my version, where you put surface definition before **END ASSEMBLY and (2) do the same as in "erode_projand_plate.inp".

Please answer me next questions:
A) Have you modified .inp file so far? Yes or no.
B) Did you submit the job? Yes or no.

So, if you did modify it, than try to submit it (it is described in my previous post). What type of error do you get in that case?


Anyway, I would need more clear explanation of the problem to help you.


Kind regards

 

[gurbuz88]

Thank you very much, finally it worked, I am very happy.

Kind regards

 

[montocristo85]

Hi,

I'm modelling erosion in 2D axisymetic model.
I followed the above steps. However, when I import the Input file (with modification of INTERIOR SURFACE), it returned me:

ValueError: omu_PrimEnum(const cow_String&) - str not allowed: INTERIOR Permissible: {S1: 100, : 111, S2: 101, S4: 103, S6: 105, END2: 109, E2: 113, E4: 115, INVALID_SURF: 116, S3: 102, SPOS: 106, END1: 108, SNEG: 107, S5: 104, E1: 112, E3: 114} This occurred while creating assembly level surface . The surface definition will be ignored.

Do you know where is this come from? (Because of 2D axisymetric model, as I know there is no restriction when using INTERIOR surface for 2D axisymetric element. Link about Interior surface:

http://server-ifb147.ethz.ch:2080/v...pt01ch02s03aus17.html#usb-int-adeformablesurf

)
I really need help, so please give me some hint.
Thank you very much.

 

[Mcakir]

Hello Everyone;
I have a similar issue,too.
Althrough I have applied the directives which trickstersson described, I haven't managed to run an analysis with no errors.

Here are steps which I followed;

I opened my cae file.
From Assembly>
Sets> (Pick Element, Name as Target)> Select all elements in target plate
Sets> (Pick Element, Name as Bullet)> Select all elements in bullet
Sets> (Pick Element, Name as eall)> Select all elements in both bullet and target
From Assembly>
Surfaces> (Pick Mesh, Name as allSurf)> Select all elements in bullet and target


Save CAE file
Jobs>Create new>Write input> then go to .inp file and edit
*Contact, op=NEW
*Contact Inclusions, allSurf,
*Contact Controls Assignment, nodal erosion=yes
*Contact Property Assignment
, , IntProp-1

And
*Elset, elset=eall
target, bullet

*Surface, type=ELEMENT, name=allSurf, eall, interior


Could you please someone help me?

 

[Mustaine3]

When you have in the .inp what you've written here, then the syntax is not correct. Some information like "allSurf" and "eall, interior" and datalines and need to be below the keyword.

Such errors are reported in the .dat


See Keyword Reference Manuals for more information.

 

[DrBwts]

I'm confused, I thought if you selected General Contact -> All with self, then any elements that are revealed due to deleted elements were automatically included in any future contact.

Is this true?

 

[Mustaine3]

No. All initial outer element faces are taken by default by the general contact. That's not updated during the analysis.

 

[Mcakir]

Dear Mustaine3 and DrBwts,
I defined General Contact and > All with Self
You are right DrBwts
Please check my file and correct me.
I checked many times but could not find any clue about solution.
Regarding the posts above I can't see anything conflicting the directive mentioned in Keywords Manual.
I suppose that there should be a mistake which is very primitive but unfortunately I havent found yet.
I added my input file for your information.

 

[Mustaine3]

It's not the contact. Your damage criteria are the source of the problem. Request DMICRT and SDEG and visualize them. The elements are heavily distorted before they are at the end of Damage Evolution and removed.

 

[DrBwts]

Have just run a few models & you are all correct about the INTERNAL elements thing.

Thanks all for the info, I had no idea this was an issue.