Different Young moduli in tension and compression

  • 222 Views
  • Last Post 01 June 2018
  • Topic Is Solved
Melchior posted this 08 May 2018

Hi!

I'm trying to do an elastic-linear model of an isotropic material that has a different Young moduli in traction and compression (25 GPa in compression, 90 GPa in traction) and i cant find a material model that allow me to do that. The elastic multilinear model doesnt let me go in compression and the cast-iron only send me error messages.

Has anyone encounterd this kind of material and if yes how did you model it?

Sincerely,

Melchior.

 

(PS : i'm on ansys version 11.0)

Order By: Standard | Newest | Votes
peteroznewman posted this 09 May 2018

Hello Melchor,

How do you know the material has different Young's Modulus in tension and compression?

Do you have test data on that?

Sincerely,

Peter

Melchior posted this 09 May 2018

Yes i made some test, and i want to approxiate the behavior with a bi-linear model (it's textile reinforced concrete)

Melchior.

 

peteroznewman posted this 09 May 2018

I can easily believe that the strength will be different in compression than tension. There are material models available that do this.

I find it harder to believe that the slope of the elastic portion of the curve is different in tension and compression. Can you share your test data? You are allowed to attach a zip file here.

Melchior posted this 09 May 2018

I dont actually have test data of one test that goes both in compression and traction, I only did tests of the composite (concrete + fiber) in traction and test of the concrete in compression (since the fiber dont have any resistance in compression) to have the two modulus. My hope was that I would be able to model the composite with one idealized material model. I guess I will have to include two different materials in my model.

peteroznewman posted this 09 May 2018

Two test, one in tension and one in compression are fine. Please share the data so we can see how different the elastic portion of each is before the nonlinear portion begins.

Melchior posted this 09 May 2018

Here is an excel file with one representative test in compression and in traction.

Attached Files

peteroznewman posted this 09 May 2018

I don't understand the Excel file.

On the compression tab, the formula to calculate Stress in column F is
(B9*1000)/(PI()*$L$3^2)
where L3 is the cylinder radius of 35 mm so I understand this is dividing force by area of the cylinder.

On the traction tab, the formula to calculate stress labeled as sigma in column E is
(1000*D10)/$M$3
where M3 is the Total Fiber Area of 35.2 mm^2 which is also force divided by area.
However, this implies a radius of 3.3 mm for a circular cross section.

I don't understand why the area changes by so much between compression and traction (tension).
Is it that the shape of the sample for traction testing is completely different than the compression sample?

Or do you mean that there are two different materials, the concrete that has been tested for compression and the fiber has been tested in a traction or tension test, without being mixed in with the concrete?

If you are separately testing two materials that will later be mixed, then to use this mixture in ANSYS, you create two materials and you have a body for the concrete and a line body for each fiber in the concrete. The fiber is called a reinforcement to the concrete. Please review this discussion for more information. Are the fibers arranged in a repeatable pattern or are they in random orientations?

Melchior posted this 10 May 2018

The area changes because it's not the same samples, in compression it's just a concrete cylinder and in tension it's a plate of concrete ( L=900mm, b = 100 mm, t = 20 mm) with fibers in it aligned in the longitudinal direction  ( 80 fibers of 0,44 mm² each in section). The fibers are in repeatable pattern but i'm using shell element with a weird shape.

Attached Files

peteroznewman posted this 10 May 2018

Thanks for the photos, that helps to see what you are doing.

The construction will have a 20 mm thick "ribbon" of fibers in concrete on the top curved surface of a cross section that will have solid concrete on the bottom curved surface of the cross section.

The test sample for tension was described above having 80 x 0.44 sq.mm fibers = 35.2 sq.mm in a concrete plate with a 2000 sq.mm cross sectional area.

When this sample is pulled, there is a steep slope for a few mm of displacement then a shallow slope. 

peteroznewman posted this 10 May 2018

Thanks for the photos, that helps to see what you are doing.

The construction will have a 20 mm thick "ribbon" of fibers in concrete on the top curved surface of a cross section that will have solid concrete on the bottom curved surface of the cross section.

The test sample for tension was described above having 80 x 0.44 sq.mm fibers = 35.2 sq.mm in a concrete plate with a 2000 sq.mm cross sectional area.

When this sample is pulled, there is a steep slope for a few mm of displacement then a shallow slope. 

peteroznewman posted this 10 May 2018

The above two posts exhibit a defect in the Add Post function of the website.  Attached is a Zip file of the content that I was trying to post, but was cut short and automatically duplicated by the website.

Attached Files

Melchior posted this 14 May 2018

Hi thanks for all your help but unfortunatly this approach wont go either. Theorically the fiber layer should be spread homogeneously in the concrete not be only at the top surface (construction wasn't easy either =) ). I expect the left and right side that are higher to be in compression and the middle part (lower) to be in tension. For the traction test it's correct that we first have a steep slope of the composite being streched until the concrete fails and then the slope of the fibers in cracked concrete.

Melchior posted this 01 June 2018

If anyone has the same problem, I managed to solve the issue by setting every element at the rigidity of the concrete, then after solving I used a macro to reduce the rigidity of the element with a stress in tension higher than the stress of fissuration. With 5 iterations like this the model converged to a final solution. For the parts where the element had traction on one side and compression on the other, i reduced the thickness to lower the stifness in flexion without lowering the stifness in compression.

peteroznewman posted this 01 June 2018

Glad to hear you had a good result!

I have been learning about different material models available in ANSYS and now know about CAST iron, which can have different stress-strain curves in tension and compression.  May be useful for another model.

Close