Seam embedded in a face (2D)

[Ffan]

Good evening to everyone.

This is my first message here and I hope I can help others the same way they help me.

I´m trying to develop an Edge cracked especimen geometry in 2D. It's a plate with dimensions 90x70x0.045mm. and it has an inclined crack in the edge (although it was applied displacement along the upper edge, vertical displacemente = 0 in the lower edge and horizontal displacement = 0 in the lower right hand corner, I think that the attached picture can provide insight).

I need to use a "seam" in Abaqus. But, in order to use it, I firstly need to draw the line of the seam in the Sketcher (modeling space: 2D planar). Because of that, I can't use the shell base feature (the most appropiate for my example, or at least that's what I think), instead I need to use the wire base feature.

So when I define the section, I tried with solid-homogeneous, shell continuum, membrane, surface... But neither of then it's possible to assign (i. e. they don't appear in the sections assignment dialog box).

I know is a quite easy example but I keep trying for several days and I can't find what I'm doing wrong. How can I do it? What sould I choose?

I´ve developed the model without the seam but the problem starts when I need to draw the line of the seam in the sketcher. And I´m not able to go further than the Sections Assignments part.

I would greatly appreciate your help.

 

[Ffan]

I forgot to say that I´ve also tried to do it by different parts.

One part will be the plate and the other one will be the seam. But,

Wich element section should I assigne to the seam? a truss? a beam?

And, how can I assembly the two parts making only one solid?

I have assembly the two parts but when I try to define the seam abaqus doesn't let me ("One or more of the selected geometric entities is an edge of a 3D region or a face of a 2D region, only interior edges of 2D regions or interior faces of 3D regions can be selected as seams").

Help is very appreciated

 

[PrntScrn]

ABAQUS can be rather .. picky where cracks are concerned.

I have always created them through the "Special" menu in the interaction module.


Define your 2D geometry first with no crack.

Sketch the crack as a partition. (It doesn't matter that it doesn't completely enclose a region for some reason it's still a partition)


In the interaction module Special>Crack>"Assign seam" and select the partition you created.

I always have to make sure I'm meshing on instance or it complains at this stage

The direction of crack propagation must be assigned so:
Special>Crack>Create
select whether you want "Contour Integral" or XEFM. (I have only ever used "Contour Integrals" so you're on your own otherwise.)

You then need to select the crack front (the tip of your crack sketch) and the direction of propagation.
Make sure you don't select the whole line for the crack front or ABAQUS will give you really weird results.

You've said and inclined crack so I'm assuming you're not using symmetry, if you are it's important to check the relevant box or you'll get bogus results when you try and calculate J-Integral, K etc.

I'd strongly recommend you have a good read through the Fracture mechanics section of the ABAQUS Manuals, to make sure you get your head round exactly what they want.

The seam doesn't get an element type assigned to it it's just where there are adjacent elements not connected to other.

To get the J-integral Stress intensity factor etc, you have to create a History output request and select "Crack" in the Domain drop-down menu.

There are some limitations on element type (basically quads only) but the error messages for these are fairly self explanatory.

A solid-homogeneous section has always worked for me, not sure why ABAQUS is complaining when you try to use it.