cancel
Showing results for 
Search instead for 
Did you mean: 

how does offset work in femap?

Creator
Creator

Hi at all, I have a question to ask about the offset feature adjust plate offset in femap. I would like to model an inclined cover and a horizontal perimeter profile. The solution gives me much less results of stress and displacement than the model withou offset. Does anyone know why this happens? I would not like femap to consider offset as a thickness and in that case my hypothesis at the base is not truthful.

Looking the deformation it seems that femap applies a spring at the offset which is reasonably less stressed on the more distant profile, but if so, I wonder how does it consider this reduction applyed to the offset and if it works like a spring as it calculates? Does it considering the properties of the plate material?

Thank you all.

FB

prova offset.jpgmodel with offset.jpgprova no offset.jpg

 

 

4 REPLIES

Re: how does offset work in femap?

Solution Partner Phenom Solution Partner Phenom
Solution Partner Phenom

Dear Franz,

This is not a problem in the FEMAP side, but of the FE solver used, FEMAP simply do the job that the user request, that is prescribing shell thickness offset in the selected elements (Shell Offset  simply consist in defining a distance between its connecting grid points and the reference plane of the element). Then double-check results, make different models with and without OFFSET, or use different elements types, compare results between shells & solids to arrive to a valid model.

I can tell you that always I can, I try to avoid offset definition. For instance, with NX NASTRAN solver the following restrictions apply:
• For linear buckling analysis (SOL105) Offsets should not be used in beam, plate or shell elements. The buckling loads for structures with offsets are incorrect.

• Offsets in the CBEAM, CTRIA3 and CQUAD4 elements are not allowed in combination with nonlinear material.

• Using 0-D scalar elements when offsets are defined on beam and shell elements will cause incorrect results in buckling analysis and differential stiffness (nonlinear SOL106 analysis) because the large displacement effects are not calculated.

• When geometry nonlinear conditions exist (PARAM,LGDISP,1), the offset vectors remain parallel to their original orientation when computing the differential stiffness. Also, when material nonlinear conditions are defined with the MATS1 or CREEP entries, the offset vectors may produce incorrect results. As a result, the specification of offset vectors is not permitted in these solutions.

• Also please note NX Nastran doesn’t modify the mass properties of an offset element to reflect the existence of the offset when you use the ZOFFS or MID4 method. If you need the weight or mass properties of an offset element for your analysis, use the RBAR method to create the offset. 

In summary, you can see that offset in many times is more a problem than an advantage: use it with caution, and double-check  results. Instead, take a look to GLUE contact, GLUE condition is supported in all solutions sequences of NX NASTRAN.

Best regards,
Blas.

Blas Molero Hidalgo, Ingeniero Industrial, Director
IBERISA • 48004 BILBAO (SPAIN)
WEB: http://www.iberisa.com
Blog Femap-NX Nastran: http://iberisa.wordpress.com/

Re: how does offset work in femap?

Creator
Creator

Thanks Blas, in my case I have a beam/plate monodimensional structure and I load only static analysis with linear material (steel and plate with stiffness that simulate corrugated shell).

what is ZOFFS and MID4 method? and How can I replicate the continuos connection with RBAR?

Since the structure is very articulated I would like to avoid a solid model so I try with a monodimensional case with beam and plate and with offset command. I use regular glue connections but only with solid modeling. At the moment I miss how I can apply the glue to my monodimensional situation.

Re: how does offset work in femap?

Solution Partner Phenom Solution Partner Phenom
Solution Partner Phenom

Dear Franz,
Not matter your loads are static your Finite Element structural model need to be prepared always to be run not only as linear static but also nonlinear static & linear buckling as well to perform a eigenvalue analysis to know the natural frequencies and mode shapes of your structure, running this way you can validate "by comparison between analysis" that your response is valid & accurate.

Without a full vision of the real whole structural problem I can't suggest the best elements to use, but beam & plate elements are the most efficient, together with rigid RBE2/RBE3 elements to define joints.

Offsetting Shell Elements
With NX NASTRAN you can offset shell elements relative to the mean plane of their connected grid points using any of three commonly used techniques to define these offsets:
• ZOFFS
• MID4
• RBAR

The method we use generally in FEMAP is ZOFFS, is a field in the CQUAD4 card that defines the prescribed Offset from the surface of grid points to the element reference plane, written element by element.

MID4 is a field of the PSHELL entry card to model laminate composite elements, and RBAR means for instance to use rigid elements RBE2 to model explicitly the offset discontinuity between Shell elements reference plane.

In summary: compare results between different meshing techniques, using locally 3-D solid CHEXA 8-nodes elements mixing together with global 2-D Shell CQUAD4 and 1-D CBEAM elements is most of the times the best meshing approach, but it depends of many factors, each real structure could be quite different ...

Best regards,
Blas.

Blas Molero Hidalgo, Ingeniero Industrial, Director
IBERISA • 48004 BILBAO (SPAIN)
WEB: http://www.iberisa.com
Blog Femap-NX Nastran: http://iberisa.wordpress.com/

Re: how does offset work in femap?

Creator
Creator
Thanks you very much Blas, now I'm adding the corrugate to beam model using midsurface and glued connection. After that I'll build solid model of the roof to compaire the results.
Thanks and see u.
FB

Inviato dal mio dispositivo Huawei