×
INTELLIGENT WORK FORUMS
FOR ENGINEERING PROFESSIONALS

Log In

Come Join Us!

Are you an
Engineering professional?
Join Eng-Tips Forums!
  • Talk With Other Members
  • Be Notified Of Responses
    To Your Posts
  • Keyword Search
  • One-Click Access To Your
    Favorite Forums
  • Automated Signatures
    On Your Posts
  • Best Of All, It's Free!
  • Students Click Here

*Eng-Tips's functionality depends on members receiving e-mail. By joining you are opting in to receive e-mail.

Posting Guidelines

Promoting, selling, recruiting, coursework and thesis posting is forbidden.

Students Click Here

Jobs

FEMAP Imposing Displacement

FEMAP Imposing Displacement

FEMAP Imposing Displacement

(OP)
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: Imposing displacement rather then applying force?
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!

RE: FEMAP Imposing Displacement

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/

RE: FEMAP Imposing Displacement

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

RE: FEMAP Imposing Displacement

(OP)
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

RE: FEMAP Imposing Displacement

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.

RE: FEMAP Imposing Displacement

(OP)
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.

Red Flag This Post

Please let us know here why this post is inappropriate. Reasons such as off-topic, duplicates, flames, illegal, vulgar, or students posting their homework.

Red Flag Submitted

Thank you for helping keep Eng-Tips Forums free from inappropriate posts.
The Eng-Tips staff will check this out and take appropriate action.

Reply To This Thread

Posting in the Eng-Tips forums is a member-only feature.

Click Here to join Eng-Tips and talk with other members!


Resources