Ship Geometry-any one can help me?
 

hi friends,
can you help me out for soughing a issue struggling me.
i made a model using solid works ,itz of a ship.i modeled it using solid works.
i can able to mesh that model in Hyper Works,but in ansys it is showing error,can you help me to find what is the error in the model.

our model is a offshore accommodation barge,we are securing a 500t lifting capacity heavy care over it.and our structure should not fail in operation.

You zip file only contains the *.wbpj file you must also include the corresponding directory which ANSYS makes that contains the geometry, mesh and simulation files.

dear Sir,
i am trying to attach those file,since the size is of too large, even after compressing.
can able to get your mail address if any.

thanks for your time and consideration

You should use the archive option in Workbench to make a *.wbpz file. To make the file small clear the generated data for the mesh and any simulations, also if you have simulations don't include the results when the dialogue box asks. Then you can upload here, may need to zip it as the *.wbpz file extension might not be accepted here.

Models
 

Dear Sir,
i have compressed the file using workbench,since the size is of too large i am uploading it on mail big file.
hear by sending the link. kindly help me

http://mbf.me/M4ofJK
http://mbf.me/88p0Uo

Regards,
Nithin

Some points that will make this easier to mesh, faster to solve and give more accurate results. The main issue is that you've got 710 parts and they are all solid (3-D) bodies and all are very thin shapes (plates and beams) .

You should spend some time in DesignModeler (DM) and make all the flat plates into surface bodies (2-D) using the Mid-Surface option in DM. I would also either make all the L-beams and I-beams which include radii into surface bodies (2-D) or better yet into line bodies (1-D) with the required cross-sections.

Using Mid-Surface surface bodies (2-D) and line bodies (1-D) will mean that the bodies will not physically touch but you sort that out with the options in the contacts such as the offset and pinball radius (Note: make sure with 2-D face to face contacts that the blue and red faces are pointing towards each other). But another option that I would do with the surface bodies is to apply in Meshing a sweep mesh method with Automatic Thin source/target and assign the solid shell element type to get rid of any gaps.

You should use the multi-body part feature in DM to reduce the number of bonded contacts. As it stands your model has 2697 auto generated contacts:eek:. Download the Mechanical training material from the ANSYS Customer Portal to read up on the details and best ways for the contacts.

A helpful hyperlink for contacts is:

http://www.simutechgroup.com/FEA/bon...nch-v14-5.html

Thank you sir,
let me go through the material,will let u kw