DamageTC3D

[cqf_2232]

Hello, I read the previous posts on the forum and saw some parameter settings about DamageTC3D. I used this ND material for the model I ran successfully before and found that it did not converge. It may be that the material parameter setting is wrong. The screenshot of the material parameter setting is as follows. There are several questions I would like to ask.
Q1: Since there is no test data, are there any recommended values for the parameters of Gt, fc0, fcr, and Gc?
Q2: The area enclosed by the stress-strain curve is the specific fracture energy, specific fracture energy * characteristic length = fracture energy. If I check automatic regularization, I need to input the value of fracture energy, then how to get the value of characteristic length, is it the mesh size of the model?
Q3: Is the Gc (integral of the stress-strain envelope after the peak in compression) defined in the opensees official website different from the Gc of DamageTC3D?

[marafini.f]

Hi!

Q1: Since there is no test data, are there any recommended values for the parameters of Gt, fc0, fcr, and Gc?

There is a lot of literature on how to describe material behavior with respect to fracture energy and the relationship between fracture energy and initial and ultimate strength. I suggest you research which approach you want to use and make some attempts. Use the material tester to see if you are obtaining the behavior that you wish for the triaxial material.

Q2: The area enclosed by the stress-strain curve is the specific fracture energy, specific fracture energy * characteristic length = fracture energy. If I check automatic regularization, I need to input the value of fracture energy, then how to get the value of characteristic length, is it the mesh size of the model?

Yes, the characteristic length is the mesh size in the model if you use the autoRegularization option.

Q3: Is the Gc (integral of the stress-strain envelope after the peak in compression) defined in the opensees official website different from the Gc of DamageTC3D?

The compressive fracture energy is the area of absorbed energy represented by the load-displacement curve due to compression load divided by the cross-section of the specimen. In DamageTC3D It should be per unit area, and it will be automatically regularized if the flag autoRegularization is flagged. Otherwise, it should be input as to specific fracture energy (per unit volume).

Enjoy your modelling
Francesca

[STKO Team]

Hello, I read the previous posts on the forum and saw some parameter settings about DamageTC3D. I used this ND material for the model I ran successfully before and found that it did not converge. It may be that the material parameter setting is wrong.

The parameters seem reasonable. Since it is a model with strain-softening, the convergence of a nonlinear problem is very hard to achieve. You can try to change the parameter "integration" from "implicit" to "IMPL-EX". It will improve the convergence, but you may need to use smaller time steps because it is a semi-explicit integration.
Also, you should change the parameters "pdf_t" and "pdf_c" to match the amount of plasticity you want. By default, we use 0 in tension (pure damage) and 0.7 in compression (both plasticity and damage). Sometimes this large difference between these 2 values can give problems. Try to use 2 values that are close to each other, something like pdf_t = pdf_c = 0.3, which is pretty good for concrete.

Q1: Since there is no test data, are there any recommended values for the parameters of Gt, fc0, fcr, and Gc?

fc0 can be 0.5*fcp
fcr can be 0.1*fcp
For the fracture energies you can use the CEB-FIB Model code:

Immagine 2020-10-26 110434.png (3.75 KiB) Viewed 6638 times

Q2: The area enclosed by the stress-strain curve is the specific fracture energy, specific fracture energy * characteristic length = fracture energy. If I check automatic regularization, I need to input the value of fracture energy, then how to get the value of characteristic length, is it the mesh size of the model?

If you check the auto-regularization you need to input the real fracture energy (not the specific). Then you don't have to worry about the mesh size because in this case, the DamageTC3D will automatically compute g = G/lch where lch is taken from each element the current material belongs to. It's done automatically.

Q3: Is the Gc (integral of the stress-strain envelope after the peak in compression) defined in the opensees official website different from the Gc of DamageTC3D?

Read this article:
https://www.researchgate.net/publicatio ... hear_walls

Immagine 2022-02-08 095801.png (25.03 KiB) Viewed 6638 times

[Lin Sun]

Dear STKO team,

I have one more question about fracture energy.

I read the above Q&A. It helps a lot. My question is about material test with DamageTC3D. For example, I need to input the fracture energy Gc and Gt (calculated from CEB-FIB equation), and selected the auto-regularization. Then I do the material test in STKO. The curve will be displacement-stress because it is not specific fracture energy.

If I want to obtain strain-stress from displacement-stress curve, I just need to divide the displacement by mesh size (characteristic length). Whenever, I change the mesh size (characteristic length), the strain-stress curve of the material will be different because I divided displacement by different mesh size. For me, it seems very contradictory and not consistent.

Could you explain more on this?

Thank you very much.

Best,
Lin Sun

[STKO Team]

You don't have to divide the abscissa by lch, only the fracture energy. Otherwise you will change also the part before the softening, hence also the initial stiffness.

What the material does internally is:

• get lch from the current finite element
• compute gt = Gt/lch and gc = Gc/lch
• compute material response with gt and gc

[cqf_2232]

Hello, I have the material code developed by myself, can STKO call it?

[Lucy2012]

Yes you can program it in python, you can check Dr. Petracca's webinars

[cqf_2232]

Dear STKO Team，
I have referenced some literature. The fracture energy is generally tensile fracture energy, but the concept of compression fracture energy has not been found. As mentioned before, gc is the area of the compressive stress-strain curve, Gc=gc*characteristic length. If I get a stress-strain curve with a 150/300 cylinder test, is my characteristic length 300mm or mesh size?
I built a 150/300mm cylinder model in compression. Enter gc (0.128) in DamageTC3D and compare it with the curve obtained from "Material Test". It is found that the curve reaches a peak and then drops off sharply. In addition, I found that there is a longer duration after the peak of the curve by entering the fracture energy (gc*mesh size=7.68).I'm very confused about this now and don't know where is the problem.

[STKO Team]

This is a topic very hard to explain in a forum post. I will talk about it in the next webinar series about RC shear walls.

However, this is what I typically do if I have an experimental stress-strain curve.

• take the area under the experimental stress-strain curve. This is called (gc) specific fracture energy (specific to the size of the specimen, in your case 300 mm)
• obtain the real fracture energy (i.e. the area under the stress-displacement curve) by multiplying the specific fracture energy and the specimen characteristic length. Gc = gc_spec * lch_spec
• In STKO use Gc and check the autoRegularization option

The autoRegularization option will compute (automatically for each element) a specific fracture energy (specific to the element characteristic length, gc_ele = Gc / lch_ele).

[cqf_2232]

I understand what you mean. The following is a comparison chart of the four cases. When I entered the fracture energy, I checked the autoRegularization.
case 1: gc=0.176
case 2: Gc=gc* specimen size (300mm)
case 3: Gc=gc*mesh size (20mm)
case 4: Gc=gc*minimum mesh size (5.2mm)
When the Gc is input, the area of the compressive stress-strain curve is obviously larger...