FEMAP Imposing Displacement

[EzequielRuizNicolini]

Hello! I am new in this forum! Im Ezequiel from Argentina. I got here because i was googleing this topic and found this thread interesting: thread1234-321413
I am trying to find stresses generated on a solid when a displacement is enforced. The solid behavior must be similar to the shown in the attached picture. I've generated the shown deformed view aplying loads instead of displacements. But what i really know is that 2mm of radial displacement must be enforced. I've tried impossing displacement at nodes of the upper feces (normal direction) but the results (also shown) are not the ones i expected. I think i am not modeling the problem in a correct way. Could you help me please?. Thank you very much!

 

[BlasMolero]

Dear Ezequiel,
You can prescribe non-zero enforced displacements in FEMAP perfectly (please note: as a loading force), but be aware that this is a large displacement effect, then geometric nonlinear analysis is required. Also, in order to avoid nastran error you need to constrains nodes exactly in the same direction (DOF) you enforced displacements.

In NX NASTRAN there are two methods available to you for specifying an enforced displacement at a component. The first method is to enter the value of the enforced displacement directly on an SPC entry.

The alternate method to enforce a displacement at a component is to use the SPCD Bulk Data entry. The SPCD entry is actually a force, not a constraint, but it is used in conjunction with an SPC entry to enforce the displacement. When you use an SPCD entry, internal forces are computed that are applied to the structure to produce the desired enforced displacements.

The SPCD method of enforcing a nonzero constraint is more efficient than using an SPC entry alone when you're using multiple subcases that specify different constraint conditions. Note also that when you use an SPCD entry, the displacement values entered on the SPC entry are ignored. The software only uses the SPCD values.

Best regards,
Blas.

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

IBERISA
48011 BILBAO (SPAIN)
WEB:

http://www.iberisa.com

Blog de FEMAP & NX Nastran:

http://iberisa.wordpress.com/

 

[rb1957]

isn't each leg of the model acting in isolation ?

what's causing the displacement ? could you model this as a force, and scale the results for your required displacement ?

Quando Omni Flunkus Moritati

 

[EzequielRuizNicolini]

Hi! Thanks for answering so fast!. I took some time because i am really new with FEMAP and FEA. I needed to "digest" all the information you brought up and study it.

Blas: Because of your answer i am still learning (found some good information) about Nastran Input Data basics. I've cheked my models input data. The one that threw me an unexpected solution i just did: Model->Load->OnSurface (picked surfaces) ->Displacement (Normal to Surfaces). The analysis Preview shows me that FEMAP auto-generated SPCD entry for the Load Set. My question: wich are the steps, if it is possible, to make FEMAP generate SPC input data that enforces diaplacement.(Firs method ypu mentioned) Thank U again!

rb1957: I did 2 differents models. As shown in the picture attached

The left-sided one, with surfaces loads. Same magnitud and normal direction to each leg "head".

The right sided one, i tried to generate a load set with the Displacement method as described above -Model->Load->OnSurface (picked surfaces)->Displacement (Normal to Surfaces)-. The "strange" bahaviour shown in the picture is what confuses me.

I think i will follow your advice and just scale the results for the requiered displacement as you said . Thanks a lot

 

[jbrackin]

In addition to creating the load>displacement>normal to surface,
did you also create constraints for those same surfaces/nodes in the radial direction in a cylindrical cord system

constraint>on surface> cylinder/hole>constrain radial growth

This will cause Femap to create a cylindrical system with its radial direction normal to your surfaces and also set the output cord system for those associated grids to this new system(this is required by nastran)

In Nastran,the direction of any enforced displacement is determined by the output cord system of the grid, doesn't matter if you use the SPCD as supported by Femap or create the input directly using an SPC entry.

 

[EzequielRuizNicolini]

Yes jbrackin! i did create those constraits. I dind't know that requierement and, initially i got ERROR MESSAGE. But i found a thread that explained me that requirement. All the same i got a strange result imposing a displacement (as shown in the picture).I decided to impose a Load that results on the desired displacement! Thank you all.