# Plane stress/strain thickness in ABAQUS

Hi there!

I have a very short question. What is the exact meaning of "plane stress/strain thickness" in ABAQUS?

It is used when section is defined for 3D models and typically takes the value of 1. I'd also like to know what difference would it make if some other value is specified. I guess, I would know that if I knew the exact meaning (or maybe not?).

### Isn't there anybody who

Isn't there anybody who knows the answer?

### hi

hello friend....

plz follow the instructions given by sir, Biswajit Banerjee comments..... i am agree with them.

good luck...

### Re: Plane stress/strain thickness in ABAQUS

I believe no one has bothered to reply because the answer can be found in any textbook on elasticity.

The keywords you should look for are "generalized plane stress" and "generalized plane strain".   A google book search gives me a link to Sadd's excellent book on elasticity  which explains the matter for the case of plane stress.  You should be able to work out the equivalent results for plane strain on your own.

Also,  plane elements can be used as plate elements if a thickness is available.   Some implementations switch over to plate elements when a thickness is specified.  I'm not sure if Abaqus does that.

-- Biswajit

Update: In ANSYS the plane stress option (without thickness) assumes that applied nodal forces are given in units of force/thickness (F/t) (where t is the thickness).  If the thickness option is chosen then the applied forces are assumed to be F and the program computes the force per unit thickness.

-- Biswajit

### Is that the correct answer?

I already knew the information contained in your answer but I think this is not was I was looking for. I am very well familiar with terms plane stress and plane strain. But, as you can see above, we have the sintagm "plane stress/strain thickness", which is not the same one, only somewhat similar. Please, pay attantion to the word "thickness" at the end. Both the plane strain and plane stress formulations are used in 2D formulations - planes, shells, where 3D field is reduced to a 2D field. Those formulations also require to define the thickness (e.g. when shell section is to be
defined in ABAQUS), but this
one ("plane stress/strain thickness") is required when the section for
3D models (solids) is defined. Hence, what is the meaning in that case? What ever it is, it is related to 3D models, and the answers should take that aspect into account.

In different tutorials you can only read to accept the default value of 1, without any further explanation what it means. I am also asking myself, what would it mean if I would define 0.1, or 10 instead of 1. I guess I'd knew that, if I knew the meaning of "plane stress/strain thickness"?

### Re: Is that the correct answer?

gaimax said

" Please, pay attantion to the word "thickness" at the end".  Indeed, that's what I was trying to address in my answer (see for instance the figure at the end of my reply).  I'm sorry that I wasn't able to answer your question to your satisfaction.

Since Abaqus is an expensive piece of software, many of us on iMechanica do not have access to it.  However, people who do have access to the software post regularly on the Abaqus Yahoo  Group or at  http://www.nabble.com/Abaqus-Users-f14343.html.  You should take your question there and also look at the user manual for the particular definition that Abaqus uses.

As I said in my previous reply, in ANSYS, the default value of 1 for the thickness indicates that the nodal forces are specified in units of force per unit length (for plane stress).  There is no equivalent thing for plane strain in ANSYS - only a generalized plane strain option.  If you define a thickness of 0.1, the applied force is assumed to be the total force and the actual force used in the analysis is f/0.1 (according to the manual).

To check that this is indeed the case, all you have to do is take a plane element, apply a small load to it, and compute the displacements.  Then apply a load 10 times as high for a plane stress with thickness element (thickness = 10) and see whether you get the same result.

Also, it helps to keep in mind that all bodies in solid mechanics are 3D whatever assumptions you might make.

Finally, a google search on your question leads me to a post pn OSdir  which says essentially what I thought was going on.  Check it out.

-- Biswajit

### Well, as I have said it, I

Well, as I have said it, I am familiar with plane strain and plain stress formulations. They are used in formulations of shells and planes. If I understand you correctly, this is what you refer to all the time - planes, shells. You are right when you say that all bodies are actually 3D bodies, hence shells and plates as well. However, planes and shells have one dimension significantly smaller than other two and this one we call thickness. So, it is clear what thickness is, and I refer to them as 2D bodies, since the formulation is mainly 2D (of course there are also 3D formulations for those bodies, but this is not the issue here).

But when I said "3D models (solids)", I meant a 3D body on which you can not make such a distinction any more! So, there is no dimension of the body which you can denote as "thickness" (e.g. a cube!). This is why I asked: what is the meaning of "thickness" in this case? This is why I emphasized this word.

I understood your answer completely, and I agree with it when it is dealt with planes or shells. You have given an example from ANSYS (BTW, I use ANSYS as well) and it is clear in that case what thickness is and what is done with the load (simply an average value over the thickness is given - that's ok). You say, in order to check your words, I just need to "take a plane element"... Well, this is exactly what I'm talking about - I am not using plane elements, I am using solid elements (hex, tetra, whatever) to model 3D bodies.

When I define section properties (it is mandatory to define them in ABAQUS, regardless what type of body you are dealing with) for a shell body in ABAQUS, I specify at first the category "Shell" (then I say it's homogeneous, this is not important), and I have to specify the value which is named thickness. That's ok, that's what I expect and I know what thickness is. Now, when I define section properties for a 3D body, at first I select the category "Solid" (once again, I say it is homogeneous), and then I need to specify a value which has the name: "plane stress/strain thickness". So, you realize this is not the thickness literally, since a 3D body (it could be a ball, or a cube, or whatever!) does not have it. I actually don't see a reason for defining this value for solids.

I have just calculated a small example in ABAQUS with a 3D body - a simple block with dimensions (axbxc) (hence, no plane nor shell) which I discretized with hex elements. I have defined external load and I have
calculated reaction forces and stresses once with "plane stress/strain thickness"
equal to 1, then again with "plane stress/strain thickness" equal to
10. in both cases I have exactly the same numbers for reaction forces and for stresses, so I couldn't see any influence of the "plane stress/strain thickness". I'm not saying there is no influence, I'm just saying it was not obvious to me and I could't see it. Is this what you expect regarding your previous answer? And, again, what is the "thickness" in a 3D body with dimensions of the same order of magnitude?

P.S. I have of course googled before I came here and I saw the post you are referring to. If I had thought that was the answer I was looking for, I wouldn't have been here. BTW, I also saw the whole post and my impression is that the person, who wrote that answer, is not an ABAQUS user.

Once again, thanks for your efforts, at least there is somebody who payed attention to my question.

### plane stress/strain thickness in Abaqus

manjunatha lakkundi
msliitr@gmail.com

1). For 3D model

a). Plane stress/strain thickness = 1

b).  Plane stress/strain thickness = 10

every results are coming same.....

''''''''''''''''''''''''''''''''''''''''''''''''''''''''''''''''''''''''''''''''''''''''''''''

2).  For 2D model

a). Plane stress/strain thickness = 1

b).Plane stress/strain thickness = 10

similarly in 2D also... same results are coming.......

Analysis done=  static  and frequency analysis

'''''''''''''''''''''''''''''''''''''''''''''''''''''''''''''''''''''''''''''''''''''''''''''''

Big question is that........  in Abaqus 3D, what is the neccessery of Plane stress/strain thickness. And I am not understanding how it is taking role in Abaqus software.

If you know plz tell me the things

### supplement

I have forgotten to write in my previous post that, in my small example with the block, the displacements were also the same with the two values (1 and 10) for "plane stress/strain thickness".

### I think it would be useful

I think it would be useful to give some additional explanation.

Namely, you stated: "
Also, it helps to keep in mind that all bodies in solid mechanics are 3D whatever assumptions you might make."

Yes, bodies are 3D, but the formulations (and therefore models) are not. Different assumptions reduce the 3D field to a 2D or even 1D field and this requires to submit additional information when you develop your model. So, I use the following terminology:

1. 1D model - e.g. rods (for truss structures) and beams - the elements have the form of lines (could be curved also) and you need  to define cross sectional area for rods, and for beams you also need to define the profile and orientation of the profile (in order to know the cros-sectional area, moments of inertia, etc.). So, the directly defined geometry of the elements is 1D and you need to define additional information about the cross section.
2. 2D model - e.g. planes and shells - you define the mid-surface and you say additionally that your body has also some thickness (this is what I mentioned above - when you specify the section you need to define the thickness). So, your geometrical model has a 2D form and the thickness is additionally defined. (I mentioned in my previous answer that there are also 3D formulations for shells (the element is referred to as "3D shell", and the "degenerated shell element" would be an example of a 2D formulation; but this is not an issue here).
3. 3D model - any 3D body (I also call this solid, therefore the misunderstanding), e.g. a cube - you use elements such as hex, tetra, wedge... - your model is a 3D model since you model the actual volume of the body and not lines or surfaces. This is where ABAQUS requires to specify "plane stress/strain thickness".

I hope it is more clear now, because I have a feeling that your answers are related to 2D models (plates, shells) only (at least your figure in the first answer is a plate - 2D model; where it is clear what the thickness is) and I am talking about 3D models. Yes, those are all solids in solid mechanics, but models are not, since various assumptions allow to reduce the full 3D field to simplified formulations and this is what I was referring to. So, my original question is related to 3D models, which are not plates, nor shells.

### I think it means...nothing.

Hi there,

I assume you're using Abaqus/CAE and defining solid sections and being prompted for the Plane Stress/Strain Thickness? You're correct that this should not have meaning for a 3D solid model. I believe that the value is not used in the simulation at all.

To quote the Abaqus/CAE User's Manual §12.2.3,

• Homogeneous solid sections. Homogeneous solid sections consist of a material name. In addition, if the section will be used with a two-dimensional region, you must also specify the section thickness. (You have the option of specifying a plane stress or plane strain thickness even if the section will be assigned to a three-dimensional region. Abaqus/CAE ignores the thickness information if it is not needed for the region type.)

and  §12.11.1

• Enter a value for the section Plane stress/strain thickness. If the section will be used with a two-dimensional region, you must specify the section thickness. Abaqus/CAE ignores the thickness information if it is not needed for the region type.

I hope this clears things up some. I admit I do not fully understand this. One way to try to confirm would be to look at the raw input files or to run some simulations and compare. I might do so myself.

Good luck and happy modeling.

### The correct answer seems to be RTFM ...

Thanks for looking up the manual.  It's quite clear that the field is ignored for 3D models in Abaqus.   So the moral of the story is RTFM.

It'll we interesting to know what Abaqus does for 2D models and whether the thickness is used in the same way as in ANSYS.

Also gagimax said " Well, as I have said it, I am familiar with plane strain and plain
stress formulations. They are used in formulations of shells and planes."  That's not quite accurate.  I'd leave it to our readers to figure out why.

Cheers.

Biswajit

### I guess that is the right answer!

@ Michael A. Graham

Finally somebody has confirmed my opinion that the value of "plane stress/strain thickness" does not come into play when it comes to 3D models. This is what I thought from the very beginning, but since it is there I decided to ask about it. As you have noticed it yourself, it is a bit confusing.

As I have tried to look up the manual (online - several times; I don't have it on the hard disc) with this specific sintagm I always had an error message saying that the page could not be downloaded (could also be a temporary problem with my internet connection), so I gave up.

And finally somebody understood correctly what I have asked and what my question referred to.

@ Biswajit

Yes, I know about RTFM and this is what I always use first (when it works). The second thing I do is "googling" and only the third thing is going to a forum (which is now for the first time, since the first two methods have always worked and are typically much faster). So, I wouldn't have been here if the first two methods had worked. And the reason why the first two methods haven't worked? For the first one, probably technical problems; for the second - I have found a number of posts with the same question, always asked by ABAQUS users, and always answered by ANSYS users in the similar way you did. The problem was that ABAQUS users didn't recognize that this is not the answer related to the topic of their question, since they were talking about 3D models as well, while ANSYS users were talking about 2D models.

Regarding "plane strain/plane stress formulations":

Please, pay attention to the fact that I have not written, that all
plate and shell elements are based on plane strain or plane stress formulation. Neither I have written that plane strain or plane stress formulation is used only for plates or shells. So, my statement was not exclusionary at any point. From that point of view I am not quite sure what you meant by saying "that's not quite accurate".The only purpose of my statement was to emphasize that my question is related to 3D models and not to 2D models, since this was obviously not understood from the beginning. Therefore, I was not aiming at being accurate on the topic "plane strain/plane stress", since it was not the topic of my question.

If we want to scratch the surface of this topic, than it would be only fair to state that majority of 2D elements in commercial FEA codes does not comply with neither plane strain, nor plane stress formulation. A great number of them is, for example, based on Mindlin-Reissner assumptions, which include transverse shear strains and stresses, which are out-of plane (e.g. "degenerated shell element", such as one I have developed in my PhD thesis for piezoelectric composite fiber-reinforced laminates)! But a plate or a shell element can be formulated so as to comply with one of those two formulations (e.g. semiloof)... This "scratching the surface" could go much further into depth, and I also leave it to interested readers, but I doubt there would be any. I am certainly not interested in this topic - first of all because I am familiar with it, then because I know where to find information on it, and finally, because it was not the topic of my question - I am glad somebody has finally recognized it and confirmed my opinion about it. But anyway, thank you for your efforts, they have probably provoked the right answer at the end.

### axisymmetric

now, does specifying plane stress/strain thickness matter for modeling an axisymmetric model?

### No. The element formulation

No. The element formulation is totally different for axisymmetric problems and specifying thickness has no meaning there.

### plane stress

plane stress condition: σzz=0

plane strain condition:εzz =0