I am using VABS to compute complex composite beam cross-section properties. The goal is then to load the properties into Abaqus and perform particular FEM simulations. Abaqus needs various cross-section properties in an input file and one of them is called "transverse shear stiffness" (GA11, GA22, GA12). I suspect it to be the elements (22, 33, 23), respectively, of the Timoshenko stiffness matrix. However, I have made some tests with simple cross-sections and I have the impression to get wrong numbers (a factor of about 1.8), unless it's actually not the transverse shear stiffness...

So, can anyone confirm that these numbers correspond to the cross-section transverse shear stiffness indeed ? Otherwise, how can I compute this ? Thank you very much.

I believe this is caused by the difference between definitions of transverse shear strains in VABS and Abaqus, which has a factor of 2. In Abaqus, they are gamma_12 and gamma_13. However, in VABS, they are 2*gamma_12 and 2*gamma_13.

Hello and thank you for your answer. So do you think I should just double the values I get from VABS ? Or is it more complicated than that for a composite beam ?

Moreover, I wanted to compare in Abaqus: a beam model (1000mm long) in which the sections come from VABS, and a solid 3D model of the same beam established in Abaqus. The section is 50mm width, 25mm height and it is divided in 3 along its height to have one different material in each part. The materials are orthotropic with "random" mechanical properties and "random" orientations (-35°, 20° and 70°). The beam is cantilevered at one tip and 100N are applied to the other tip.

The problem is that I always get about 10% of difference between the two cases, even when I refine the meshes or take a longer beam. Do you have any idea of where it can come from ? Thanks for you help !

Raphaël

EDIT : I also generated the same model in GEBT, using VABS properties, and the results in terms of deflection at tip are the following :

After checking the Abaqus documentation, I found that for the effective transverse shear stiffnesses, Abaqus calculates GA firstly by simply summing the product of shear modulus and area of each element. Then a shear factor is used to calculate the final effective transverse shear stiffness. However, for meshed sections in Abaqus, the factor is always 1, which is incorrect, even for a simple rectangular cross section (Abaqus does not know it is rectangular if it is a meshed section). Hence the results are not reliable. For more details, you can check the Abaqus Analysis User's Guide 29.3.3 Choosing a beam element and Abaqus Theory Guide 3.5.6 Meshed beam cross-sections.

Regarding to the comparison between VABS/GEBT and Abaqus 3D solid model, I would suggest to compare results from the interior part of the structure, e.g. a middle point. Also, you can recover the displacements of the original 3D structure using VABS first and compare the results at the exactly same location between the two methods.

Raphael Nardin@ on — Edited @ onHello everyone,

I am using VABS to compute complex composite beam cross-section properties. The goal is then to load the properties into Abaqus and perform particular FEM simulations. Abaqus needs various cross-section properties in an input file and one of them is called "transverse shear stiffness" (GA11, GA22, GA12). I suspect it to be the elements (22, 33, 23), respectively, of the Timoshenko stiffness matrix. However, I have made some tests with simple cross-sections and I have the impression to get wrong numbers (a factor of about 1.8), unless it's actually not the transverse shear stiffness...

So, can anyone confirm that these numbers correspond to the cross-section transverse shear stiffness indeed ? Otherwise, how can I compute this ? Thank you very much.

Raphaël

Su Tian@ on — Edited @ onHello Raphael,

I believe this is caused by the difference between definitions of transverse shear strains in VABS and Abaqus, which has a factor of 2. In Abaqus, they are gamma_12 and gamma_13. However, in VABS, they are 2*gamma_12 and 2*gamma_13.

Su

Raphael Nardin@ on — Edited @ onHello and thank you for your answer. So do you think I should just double the values I get from VABS ? Or is it more complicated than that for a composite beam ?

Moreover, I wanted to compare in Abaqus: a beam model (1000mm long) in which the sections come from VABS, and a solid 3D model of the same beam established in Abaqus. The section is 50mm width, 25mm height and it is divided in 3 along its height to have one different material in each part. The materials are orthotropic with "random" mechanical properties and "random" orientations (-35°, 20° and 70°). The beam is cantilevered at one tip and 100N are applied to the other tip.

The problem is that I always get about 10% of difference between the two cases, even when I refine the meshes or take a longer beam. Do you have any idea of where it can come from ? Thanks for you help !

Raphaël

EDIT : I also generated the same model in GEBT, using VABS properties, and the results in terms of deflection at tip are the following :

- Abaqus, beam model : 14.87mm

- Abaqus, solid 3D model : 16.44mm

- GEBT : 17.35mm

Where do these differences come from ?

VABS input file, run to get the properties used in Abaqus for the beam model

131 KBClick to download

Su Tian@ onHi Raphael,

After checking the Abaqus documentation, I found that for the effective transverse shear stiffnesses, Abaqus calculates GA firstly by simply summing the product of shear modulus and area of each element. Then a shear factor is used to calculate the final effective transverse shear stiffness. However, for meshed sections in Abaqus, the factor is always 1, which is incorrect, even for a simple rectangular cross section (Abaqus does not know it is rectangular if it is a meshed section). Hence the results are not reliable. For more details, you can check the Abaqus Analysis User's Guide 29.3.3 Choosing a beam element and Abaqus Theory Guide 3.5.6 Meshed beam cross-sections.

Regarding to the comparison between VABS/GEBT and Abaqus 3D solid model, I would suggest to compare results from the interior part of the structure, e.g. a middle point. Also, you can recover the displacements of the original 3D structure using VABS first and compare the results at the exactly same location between the two methods.

Hope these are helpful.

Best regards,

Su

Raphael Nardin@ onYes it is, thank you for your answer !

Raphaël