Register to reply

ANSYS - modeling

by lskrinjar
Tags: ansys, modeling
Share this thread:
lskrinjar
#1
Apr14-10, 03:58 AM
P: 2
I would like to model in ansys a one-half of a ring with variable cross-section.

What is the easiest way to define variable cross-section for elements in ansys?
Do I have to define 5 (for example) different cross-section for each of 5 elements, if I create 5 beam element with different cross-sections and other section properties?
Can I import the table of cross-section and then somehow link it with the element type properties? Which element type can I link with the imported table?

I don't know with wich element types does function preprocesor-sections-beam-... work.

Thanks for your help!
Phys.Org News Partner Science news on Phys.org
Wildfires and other burns play bigger role in climate change, professor finds
SR Labs research to expose BadUSB next week in Vegas
New study advances 'DNA revolution,' tells butterflies' evolutionary history
minger
#2
Apr14-10, 12:13 PM
Sci Advisor
P: 1,498
Are the cross-sections step change? Either way, here's what you'll do
  • Enter cylindrical coordinate system, CSYS,1
  • Create keypoint at 0,0
  • Create keypoints at each point where the cross section changes, and the end. You should have 6 total keypoints over the semi-circle
  • Join these keypoints with arcs, LARC,kp_start,kp_end,radius

You now have the geometry. You'll next need to create your materials and cross sections. Here's where the step or linear change comes into play. If your cross sections are simply step changes, then simply define each cross section, for a total of 5 cross-sections. It will look something like this:
SECTYPE,1,name,BEAM,beam_type,refine_key
SECDATA,CIRC,0.4,10,10,2
That is, if you're lucky enough to have your cross-sections definable by the beam cross sections. If they are arbitrary cross sections, then you can import your cross-sections as IGES or whatever, and mesh them using MESH200 element types. Finally I believe there is a command called SECWRITE, which will write out a section data file. Then, you're command for each section will look something like:
SECTYPE,1,name,MESH
SECREAD,file,sect
*Note that syntax is probably messed up so consult the guide.

Now.....if your cross sections are not step changed, but if they are similar shape but taper themselves, then you can use TAPER beam sections. For a taper section, you define the starting cross-section and the ending cross-section, and then define an additional cross-section with a taper type. It will look something like this:
SECTYPE,10,name,BEAM,beam_type,refine_key
SECDATA,CIRC,0.4,10,10,2
SECTYPE,11,name,BEAM,beam_type,refine_key
SECDATA,CIRC,0.8,10,10,2
SECTYPE,1,name,TAPER
SECDATA,10,11
Again, I'm not sure about the syntax, but basically the TAPER SECDATA simply defines the two cross sections that you want to use. Actually, there are coordinates in there as well. Starting and ending coordinates. It is important when using TAPER sections that you follow your meshing up with an /ESHAPE,1 to make sure everything looks OK. Taper sections can be a little bit of a pain in the ***.

Finally, simple mesh over the lines with the appropriate BEAM element type to generate the elements. IIRC, there is a BEAM183, so create your beam element type, and then you can just change your section in a DO loop or something, ala:
TYPE,1
REAL,1
MAT,1
*DO,i,1,5
  SECN,i
  LMESH,i,i+1
*ENDDO
Hope this helps, good luck!


Register to reply

Related Discussions
Get a copy of ANSYS? Mechanical Engineering 1
Need help with ANSYS Mechanical Engineering 16
Ansys tutorials based on harmonic analysis Mechanical Engineering 4
Who use ANSYS ? Mechanical Engineering 4
Ansys HELP General Engineering 4