×
INTELLIGENT WORK FORUMS
FOR ENGINEERING PROFESSIONALS

Log In

Come Join Us!

Are you an
Engineering professional?
Join Eng-Tips Forums!
  • Talk With Other Members
  • Be Notified Of Responses
    To Your Posts
  • Keyword Search
  • One-Click Access To Your
    Favorite Forums
  • Automated Signatures
    On Your Posts
  • Best Of All, It's Free!
  • Students Click Here

*Eng-Tips's functionality depends on members receiving e-mail. By joining you are opting in to receive e-mail.

Posting Guidelines

Promoting, selling, recruiting, coursework and thesis posting is forbidden.

Students Click Here

Jobs

internal surfaces - perforation problem
2

internal surfaces - perforation problem

internal surfaces - perforation problem

(OP)
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?

RE: internal surfaces - perforation problem

just write the input file (job, write input file) and add them in a text editor?
and what do you mean you can not add lines under surface in input file?

RE: internal surfaces - perforation problem

(OP)
Sorry if i was not clear enough

i modify input file in keyword editor (in Abaqus CAE go to Model -> Edit Keywords).

When i write additional lines under *SURFACE keyword and click OK Abaqus gives me message:
"New lines may not be added to the following keyword *SURFACE, TYPE=ELEMENT, NAME=ERODE"

I have been modifying input file with keyword editor before and it was working fine (for example *IMPERFECTIONS, *MODEL CHANGE,...). I suppose it is the same effect as modifying input file in a text editor...

RE: internal surfaces - perforation problem

2
(OP)
I finally found out a solution of my problem. I guess it is appropriate to share it with you:

1. The main problem when modeling penetration/perforation (impact analysis) or also chip formation (milling, drilling,... analysis) is to define INTERNAL SURFACES. During analysis elements on the surface fail and internal elements are exposed to contact.
2. Internal surfaces CAN NOT be set in Abaqus/CAE.
3. Internal surfaces CAN NOT be set in Keyword editor (in Abaqus/CAE: Model->Edit Keywords)
4. Internal surfaces must be defined directly in INPUT FILE (.inp) with text editor.


This is how I solve the problem:
1. I created model geometry, material properties, boundary conditions and everything else in Abaqus/CAE and created an input file.
2. I opened the input file with text editor (notepad ++) and add additional lines to define INTERNAL SURFACE:
before *End Assembly I inserted:

*SURFACE, TYPE=ELEMENT, NAME=SURF1
,
ERODE, INTERIOR

(where SURF1 is any name you choose to name internal surface and ERODE is an element set containing all the continuum elements of perforated part - this should be defined in Abaqus/CAE)

3. I defined contact (for this type of problem general contact should be used):

*CONTACT, OP=NEW
*CONTACT INCLUSIONS
SURF1, (SPHERE)
...

(SPHERE is the name of the surface that is penetrating through the material or is cutting the material. You can also live the line empty after comma. It should still work fine)
4. Submit the job and enjoy the results :)


I uploaded some tutorials you may find useful. There is also 2 examples in Abaqus Example Problems Manual:
a) 2.1.3 Rigid projectile impacting eroding plate
b) 2.1.4 Eroding projectile impacting eroding plate

RE: internal surfaces - perforation problem

(where SURF1 is any name you choose to name internal surface and ERODE is an element set containing all the continuum elements of perforated part - this should be defined in Abaqus/CAE)

Do you mean both SURF1 and ERODE should be defined in Abaqus/CAE or just ERODE ?

Also when I submit the job it overwrite on the already existing file , how can I avoid that run the amended file?

Thank you very much

RE: internal surfaces - perforation problem

(where SURF1 is any name you choose to name internal surface and ERODE is an element set containing all the continuum elements of perforated part - this should be defined in Abaqus/CAE)

Do you mean both SURF1 and ERODE should be defined in Abaqus/CAE or just ERODE ?

Also when I submit the job IN Abaqus/CAE it asks me if I want to overwrite on the already existing file and i only have the choice of clicking OK or Cancel, how can run the job file and at the same time keep the changes I made in the input file

Thank you very much

RE: internal surfaces - perforation problem

(OP)
Hi!

Only ERODE should be defined in Abaqus/CAE.

I am not sure if I understand your second question correctly, but anyway, this may help:

If you are submitting a job in Abaqus/CAE, then you have to create a new job if you do not want to overwrite already existing files. In Create Job window choose name for the job, and then set your input file as an source.

If you are submitting a job in Abaqus Command environment then you should use:
abaqus job=job_name (choose name for the job)
press Enter, then you will be asked to specify input file. Write it, press Enter and your job will be submitted.


Cheers

RE: internal surfaces - perforation problem

Hi trickstersson , I tried what you mentioned but it did not work for me :( ,I will tell you what I did exactly:

in the plate part I defined the following

Set--> type : element then selected the whole plate and named it ERODE

then I opened the input file and before *End Assembly I inserted:

*SURFACE, TYPE=ELEMENT, NAME=SURF1
,
ERODE, INTERIOR

then I defined a general contact as shown below

*CONTACT, OP=NEW
*CONTACT INCLUSIONS
SURF1,

then submitted the job but it is not working , am I doing something wrong here ?

thanks a lot


RE: internal surfaces - perforation problem

(OP)
Hi!

Did you mesh your plate first? I think you should first mesh it in mesh module. Than create set (choose element set as you did) and than choose all elements in plate.

This is one thing that could go wrong. But of course there could be many other things. Can you tell me more about your model? What problem do you model? Is that machining, drilling or impact? Do you have high velocity or low? Which constitutive model do you use for plate?

The best thing I can recommend to you is to check your output files (.dat, .msg,.stat) for warnings and errors. Than you will know where is your problem (maybe contact is not a problem at all but rather constitutive model).


Feel free to ask if there will be anything I can help with.


Cheers

RE: internal surfaces - perforation problem

Hi trickstersson,

sorry for the late reply, I have managed to get over this problem by using surface to surface contact and it worked fine for my models, I am modelling drilling process, but I think I should also learn how to do this in the way you described to me , I have tried many times before but it did not work :

I did the following in the input file: this is just a part of my input file and with modification


** Constraint: Constraint-1
*Rigid Body, ref node=_PickedSet90, elset=_PickedSet91
*SURFACE, TYPE=ELEMENT, NAME=SURF1
,
ERODE, INTERIOR

*End Assembly
**
** MATERIALS
**
*Material, name=Al2024


and inside Abaqus CAE I defined an element set named INTERIOR and defined a mesh surface named SURF1.

could you please tell me if I have missed something here

Cheers

RE: internal surfaces - perforation problem

if i modify the input file and then run it through abaqus CAE and then create a new job, the new input file created does not have the additional lines which I added before?? how can I avoid this problem

RE: internal surfaces - perforation problem

(OP)
Hi!

1. I think you must choose element set in MESH MODULE, and name it ERODE. You do not have to define nothing with name SURF1. Just leave this name as it is.

2. When you will create a new job, a pop-up window will be shown with name: CREATE JOB. Under a Name you write any name. In next line you choose Source. You have ONLY TWO options: either Model in Abaqus CAE or Input file. I think you made a mistake here. You should choose Input file as a source and then add link to your modified input file (modified in text editor).


Cheers

RE: internal surfaces - perforation problem

Hi ,
I am simulating the same process like you and I faced some problems in my modelling. One of the problems is that the tangential and normal forces in 3D are much lower than 2D. I think that there is a problem in contact of 3D.
I tried to follow your method, but it does not work. Please let me know what I need to do.

Cheers

RE: internal surfaces - perforation problem

(OP)
Hi imanjoon!

Can you tell me in what exactly does not work? How far are you with your model and what are you trying to simulate?

I do not know much about tangential and normal forces in contact, I was not interested in those forces.

Kind regards

RE: internal surfaces - perforation problem

Hi trickstersson,

I am modeling the scratch test of elastic-plastic material in 3D model. I am using the same process you mentioned. But I faced an error that it does not run the job.

RE: internal surfaces - perforation problem

(OP)
Hi Rostamsowlat!

I am afraid that I can not answer you because you did not provide enough informations about your model. A lot of things can cause an error when you submit the job.

Maybe we will be able to help you if you will give us more informations, for example:
1. Is your model 2D or 3D
2. Is the object creating a scratch ideally rigid or also elasto-plastic?
3. What about contact model (is it simple as in my case or did you use other contact definition?)
4. What did you model so far and where your model stops?
5. Did you check output files for error messages (.log, .msg, .dat,...)?
6. Boundary conditions?

Best advice that I can give you at the moment is, that in that kind of problems you should work step by step. First create very very simple model, and than include more complexity in few steps.

Kind regards



RE: internal surfaces - perforation problem

Hi tricktersson I define everything properly, then create a job before submitting and choose write input. Later I find the inp. file in abaqusworkingfiles add surface and contact definitions, save the file. I return the job file bit it gives errors. can you help me?

RE: internal surfaces - perforation problem

(OP)
Hi Gurbuz88!

Did you submit new .inp file (where surface and contact definitions have been added) or did you submit model created in Abaqus? You have to open job manager -> Create -> than choose modified input file as a Source.

Can you give us more information about the error? What type of error do you get (check log and msg files)?

Kind regards

RE: internal surfaces - perforation problem

Hi tricktersson thank you so much for your nice respond. I define everything properly, then create a job before submitting and choose write input. Later I find the inp. file in abaqusworkingfiles add surface and contact definitions,(But here the format of inp. file is different from the given erode_projand_plate.inp: For example: you say that I add surface definitions before *End Assembly but in the erode_projand_plate.inp, surface definitions are different location. So I could not cope with is problem. Thank you


RE: internal surfaces - perforation problem

(OP)
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

RE: internal surfaces - perforation problem

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

Kind regards

RE: internal surfaces - perforation problem

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/v6.14/books/usb/... )
I really need help, so please give me some hint.
Thank you very much.

RE: internal surfaces - perforation problem

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?

RE: internal surfaces - perforation problem

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.

RE: internal surfaces - perforation problem

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?

RE: internal surfaces - perforation problem

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

RE: internal surfaces - perforation problem

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.

RE: internal surfaces - perforation problem

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.

RE: internal surfaces - perforation problem

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.

Red Flag This Post

Please let us know here why this post is inappropriate. Reasons such as off-topic, duplicates, flames, illegal, vulgar, or students posting their homework.

Red Flag Submitted

Thank you for helping keep Eng-Tips Forums free from inappropriate posts.
The Eng-Tips staff will check this out and take appropriate action.

Reply To This Thread

Posting in the Eng-Tips forums is a member-only feature.

Click Here to join Eng-Tips and talk with other members!


Resources