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?

 

[burningDiesel]

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?

 

[trickstersson]

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...

 

[trickstersson]

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

 

[trickstersson]

Another useful tutorial

 

[khalchris]

(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

 

[khalchris]

(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

 

[trickstersson]

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

 

[khalchris]

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

 

[trickstersson]

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

 

[khalchris]

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

 

[khalchris]

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

 

[trickstersson]

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

 

[imanjoon]

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

 

[trickstersson]

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

 

[Rostamsowlat]

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.

 

[trickstersson]

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

 

[gurbuz88]

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?

 

[trickstersson]

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

 

[gurbuz88]

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