Drilling Degree of Freedom for Plate / Shell Elements 5

[JoshPlumSE]

I thought I learned (way back in my college days) that the "drilling degree of freedom" for plate elements was not included in a proper plate / shell element formulation. As a work around, I have always drawn in a series of frame elements at that location to convert the drilling moment into in-plane forces on the mesh of shell elements.

But, more recently, I've been exposed to a number of programs that now include the drilling DOF as part of their formulation. Programs that are widely used and which I respect.

Can someone explain to me what I'm missing?

Is this truly a robust handling of that degree of freedom? Or, is this merely a "back door" method of preventing instabilities for membranes? Where we really still have to use the in this direction, but where we still have to use the frame element work to get truly accurate results?

 

[Mohanlal0488]

Hi JoshPlumSE

The aspect of "drilling" does not form part of your plate element formulation it replaces rotational/translational stiffness's in a specific direction by a "stiffness multiplayer" which will effectively suppress drilling degrees of freedom.

The basic idea is that solver extracts two 3x3 sub-matrices from the global stiffness matrix, one sub-matrix for the translational degrees of freedom and another for the rotational degrees of freedom. The rows and columns in each sub-matrix correspond to the stiffness values at the node. The sub-matrices are used to perform checks so that a solver can flag rotational or transnational singularities.

I tend to develop models where such functionality does not need to be used as there are cases where the formulations may not work correctly, this however is mainly in non-linear analysis.

I hope that this helped in some way and that my interpretation is correct.

 

[rb1957]

in the olde days (that I, and maybe you too) can remember, I thought the issue was that the element formulation had no stiffness in the MZ so you had to constraint it (to prevent NASTRAN having a nervous breakdown over "0/0". Then to save the user constraining all these freedoms NASTRAN said, "we'll save you the trouble and create AUTOSPC, and this will be good". Well, the law of good intentions hit that one hard. Newer element formulations may have a stiffness for MZ … try them out in a single element patch test.

another day in paradise, or is paradise one day closer ?

 

[BlasMolero]

Dear Josh,
For you to know in the FEMAP & Simcenter NASTRAN suite from SIEMENS the CQUADR & CTRIAR elements are improved plate elements: for instance, CQUADR is a quadrilateral isoparametric plate element with no coupling of bending and membrane stiffness; the membrane stiffness formulation includes rotation about the normal to the plane of the element.

The CQUADR & CTRIAR take advantage of the normal rotational degrees of freedom (which have no stiffness associated with them in the standard plate elements) to provide improved membrane accuracy. The Simcenter NASTRAN software computes a rotational stiffness about the normal to the element at the vertices, which is used in the formulation of the element stiffness. Consequently, this degree-of-freedom must not be constrained unless it occurs at a prescribed boundary.

When compared to the regular CQUAD4 and CTRIA3 elements, the CQUADR and CTRIAR are much less sensitive to high aspect ratios and values of Poisson’s ratio near 0.5. For example, the CQUADR element provides better performance for modeling planar structures with in-plane loads than CQUAD4.

Best regards,
Blas.

~~~~~~~~~~~~~~~~~~~~~~
Blas Molero Hidalgo
Ingeniero Industrial
Director

IBERISA
48004 BILBAO (SPAIN)
WEB:

http://www.iberisa.com

Blog de FEMAP & NX Nastran:

http://iberisa.wordpress.com/

 

[rb1957]

interesting … how do you specify CQUADR in lieu of CQUAD4 in FeMap ?

another day in paradise, or is paradise one day closer ?

 

[BlasMolero]

Hello!,
Is very easy, in the NASTRAN BULK DATA OPTIONS of your analysis make sure to activate ALL PLATES AS CQUADR/CTRIAR, then all plate elements in the model will have rotational stiffness in the direction normal to the plane of the ele­ment.

Best regards,
Blas.

~~~~~~~~~~~~~~~~~~~~~~
Blas Molero Hidalgo
Ingeniero Industrial
Director

IBERISA
48004 BILBAO (SPAIN)
WEB:

http://www.iberisa.com

Blog de FEMAP & NX Nastran:

http://iberisa.wordpress.com/

 

[rb1957]

thx Blas !

another day in paradise, or is paradise one day closer ?

 

[nlgyro]

Coming back to some of the questions the OP has posted:

> Is this truly a robust handling of that degree of freedom?

The answer is NO. The simplest way to verify this is intentionally load the drilling d.o.f and measure its response.

The classic problem to do this is the flagpole model.

A flagpole modeled as a cbeam element is attached to the base structure modeled using shells. The cbeam/shell interface has a common node (meaning the structure is welded)

A torque(Mzz) is applied to the free end of the cbeam which is transmitted to the shell as a drilling moment. The nodal rotation (Rz) at the beam/shell interface is studied for various mesh densities on the shell.

The following is the summary:

As you can see the model diverges and a stable solution cannot be obtained. The modeling has been done using Simcenter Nastran 2019.2. MSC/Nastran 2020 also yields similar results. So one still needs to be careful in transmitting drilling moments onto shells with in-plane rotational d.o.f's.

> Or, is this merely a "back door" method of preventing instabilities for membranes?

It looks like it as can be seen from the flagpole model a stable solution cannot be obtained once the drilling d.o.f is loaded.

> Where we really still have to use the in this direction, but where we still have to use the frame element work to get truly accurate results?

One place where the use of cquadr's benefits greatly over the standard cquad4 is modeling membrane behavior using coarse grid fem's. The classic McNeal-Harder beam test problem (as shown below) is taken as an example case:

The loading being studied here is an in-plane moment applied as a force couple at the free end. The results presented here are the tip deflections normalized to the theoretical value.

But if you run into applications where you have to transmit drilling loads into shells you still need to transform the moments to force couples by "spidering" out to adjacent grids using beams, rigid elements (rbe3, rbe2). IMHO!!

 

[rb1957]

anyone putting that much work into a response deserves a LPS !

excellent job !

another day in paradise, or is paradise one day closer ?