Gap elements with Femap
Wytze Hoekstra
experience with this program (we don't have much experience with FEM
in general. I have done some simple static analysis that worked fine
(parts for hydraulic presses and injection units). Recently I read
something every interseting about gap elements. I have tried to use
this thes gap elemnts to model contact surfuces between to parts, but
without any succes. I have been busy for a few days now and I tried
everything, but it doesn't seem to work. We are using CSA/Nastran
(version 94) as processor. Are there any examples available on the
web? Can somebody send me an simple example by e-mail? Can somebody
explain how these elemnts work? Any help would be aprecciated. (We
also have a test version of femap 7.1, so I can open 7.1 files to
study them.
Wytze Hoekstra
w.hoe...@vdploeg.nl
Jeff Finlayson (w)
CGAP cards. Take a look at the CSA/Nastran user's manual if you have
one. I'll give you some more info when I have time. Good luck.
Jeff Finlayson
Boeing
Huntsville, Alabama
Jeff Finlayson (w)
having? Such as model won't run, or strange warning messages.
Jeff out ...
Wytze Hoekstra
> You said you haven't had any success. What problem(s) are you
> having? Such as model won't run, or strange warning messages.
Today I finally have succesfully done a very simple example:
(http://www.mechsolutions.com/support/online_ex/Nastran/Nas105/workshop_30c.pdf)
The model works fine but I still don't understand exactly why. I Think
something went wrong when defining the element properties. The
following I don't understand:
- What influence has the "Transverse Stiffness" and can I use a zero
value here
- Do I have to use "Interface Element Normal" and what does this mean?
- What is "Interface Widht or Area"
When defening the gap element Femap asks for two nodes and an
orientation vector. I don't know how to choose the orientation vector,
in the example I used 1,0,0 and that worked fine but I don't know why.
Wytze
Jeff Finlayson (w)
is closed. The MSC/Nastran manual says its default is Mu*Ka.
Mu is the coefficient of friction for the sliding surface. Ka is the
axial stiffness of the closed gap. The MSC manual recommends that
Kt >= 0.1*Ka. These are defined on the PGAP nastran card.
The element normal should be normal to the sliding/contact surface.
1,0,0 is the x axis. The contact surface should be the YZ plane then.
Hope this helps.
Jeff out ...
Wytze Hoekstra
> The transverse stiffness (Kt) is the sliding stiffness when the gap
> is closed. The MSC/Nastran manual says its default is Mu*Ka.
> Mu is the coefficient of friction for the sliding surface. Ka is the
> axial stiffness of the closed gap. The MSC manual recommends that
> Kt >= 0.1*Ka. These are defined on the PGAP nastran card.
>
> The element normal should be normal to the sliding/contact surface.
> 1,0,0 is the x axis. The contact surface should be the YZ plane then.
>
> Hope this helps.
>
> Jeff out ...
>
Thank you, I finally start to understand the gap element. One more
quaestion about the element normal, what if the contact surface is not
a plane but a cilindrical surface, e.a. an shaft in a hole:
http://www.engr.udayton.edu/faculty/dmyszka/WebPages/mct446/Gaps.pdf
Jeff Finlayson (w)
coord. system for the grids (reference and analysis). Also use c.s.
to define the element direction vector. Use a (1,0,0) for the radial
direction. Or set up a rect. c.s. for each gap element (takes a while).
Jeff Finlayson
Boeing
Huntsville, Alabama
Wytze Hoekstra
> For a cylindrical contact surface use the a cylindrical
> coord. system for the grids (reference and analysis). Also use c.s.
> to define the element direction vector. Use a (1,0,0) for the radial
> direction. Or set up a rect. c.s. for each gap element (takes a while).
>
> Jeff Finlayson
> Boeing
> Huntsville, Alabama
Thank you very much, I think I understand the concept of the gap element now.
Wytze