×
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

Thermal Expansion and Poisson ratio

Thermal Expansion and Poisson ratio

Thermal Expansion and Poisson ratio

(OP)
If I simulate the thermal expansion of a square sheet with Abaqus, I receive an expansion that is too large by the Poisson number.
E.g. a simple set up:
A 1x1 square sheet, with a thermal expansion coefficient of 1E-6 and a temperature increase of 1000 degree should expand by 1E-3. Instead I receive an expansion of 1.3E-3 if the Poisson ratio is set to 0.3.

Can anybody give some enlightenment? Or am I fooling me myself???
cheers, Daniel

RE: Thermal Expansion and Poisson ratio

..should increase by 1e-3, instead I receive an expansion of 1e-3? Have I misread this somewhere?

RE: Thermal Expansion and Poisson ratio

(OP)
note that the expansion is: 1.3e-3, not 1e-3!!!!

I think I found the reason for the extensive expansion. In a 2dim Model, Abaqus seems to keep the third dimension constant! Due to the thermal expansion, the 3.dim would expand by 0.001xlength. With a length of 1 this would give 0.001. Keeping it constant results in compressing it by 0.001. With a Poisson ratio of 0.3 this results in an additional expansion along the first dimension by 0.0003, exactly what I observe.
Now, I am new to Abaqus and you may help me understand, where the constant third dimension is defined. The only thing I found is in the "Edit Section" dialog, where there is an entry "Plain strain/stress  thickness". But I did not check this!
cheers, Daniel

RE: Thermal Expansion and Poisson ratio

My fault. The problem with 2D thermal stresses is that you need generalised plane strain where free expansion out of plane is allowed. You have defined plane strain, with zero strain. Change the element type, define a reference point, and restrain that so that only the rotational freedoms of the plane are restrained. For that you need to manually edit the inp file as you can' do it in CAE.

RE: Thermal Expansion and Poisson ratio

(OP)
I finally succeeded,thank's a lot for your help.
One last question. I did the thermal expansion because I did not succeed in modeling an interference fit. It works now, but it looks like a rather clumsy way for doing it. Is there not a more elegant solution? And why is it so difficult to model an interference fit directly?
cheers, Daniel

RE: Thermal Expansion and Poisson ratio

Two ways of modelling interference is to use thermal expansion as you have done, and secondly to impose an interference fit directly in the interaction module. There's an option in the contact set up to include this.  

RE: Thermal Expansion and Poisson ratio

(OP)
I tried the direct way first, but had troubles with convergence. That is why I tried thermal expansion. Can I find an example of an interference fit somewhere?
cheers, Daniel

RE: Thermal Expansion and Poisson ratio

Hello Daniel,
I am doing interference fit on a model using ABAQUS CAE and have been successful with it. However, now I want to try using temperature approach that you mentioned.
Can you please tell me how did u go about it? I have changed the material properties to include the thermal coefficient but am not sure about the boundary conditions and loading.

Regards

RE: Thermal Expansion and Poisson ratio

(OP)
Hi Ashu28,
unfortunately I do no more have these calculations I. But I prepared an example, OneCyl.cae,  for you. I try to upload it.
OneCyl is a simple cylinder that get heated from 0 to 100 degree and  threfore expands.
Points to pay attention:
-Element type: Coupled Temperature Displacement
-Analysis type: Generalized plain strain
-Temperatures can be specified in boundary conditions.
- Convergence is difficult, therefore use damping e.g.: Automatic stabilization (see under "step")

I then made a second example, TwoCyl,  with two concentric cylinder. The inner cylinder is then heated and expands, creating an interference fit. On a first view this seems to work, but the grids on both cylinders interpenetrate. Beeing pretty new to Abaqus, I did not yet find out what is wrong here. This itches, because last time this did not happen.

I would like to learn how to make an interference fit. Could you please send me an example.

cheers, Daniel
 

RE: Thermal Expansion and Poisson ratio

Hello everybody

I have problem to simulate cooling a a part
my part include 2 section, material of top section is Aluminum and Material of bottom section is Copper and these part are welded together
the initial temperature of this part is 433K,
This part quench during 1 second and final temperature is 298K

Please help me to simulate this problem
 

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