Importing assembly - joining of parts 1

[Fotzio]

I have a problem. I imported assembly with few parts to Abaqus, and some of parts have to be joined (to form the same deformable solid). How can I join different parts keeping them as volume partions, so I can later get structured mesh?
Thanx for any help!

 

[brep]

In the assembly module you can use the merge parts (Boolean) feature. Note there is a checkbox whereby you can keep the internal faces.

Otherwise, if you just have one volume (cell) you can use the many partitioning tools to subdivide the cell into multiple structured/sweep meshable cells. (There have been many improvements made in V6.6 to sweep meshing that make it much more forgiving to your topology)

 

[brep]

Extra bonus tip:

For those of you who think you've exhausted the partitioning options (even though there are quite a few), there is a nice trick you can play:

To partition a cell, you can actually create a shell feature (extruded, revolved, lofted, etc) and look at the dialog box before you finally create it. There is a check box to say "keep internal faces". This will have the effect of "partitioning the cell. I find this particularly useful with the shell loft when the shape of the partition you want to make is quite difficult...

Finally, as one more bonus:
You can actually make multiple partitions at the same time. Just try it with extruded shells (sketch a whole bunch of circles to create extruded "tubes". Use the "keep internal boundaries" checkbox, and watch what happens!

 

[Fotzio]

Thank you brep for your fast and very helpful advice. I managed to merge parts and keep partitions.
I need one more advice. How to solve incompatibility between regions? When meshing some partitions I get warning message that incompatible mesh (incopatible element shapes) will be created. It is transition from structured to free meshed region.

 

[brep]

You can try to make both regions hex meshable (structured and/or sweep), or you can accept the incompatible mesh info message, which is actually fine if you don't mind having a tie constraint in there. (Tie constraints used to be a dirty word in FEM, but ABAQUS has some specific technology to make such constraints much more acceptable these days)

 

[Fotzio]

Brep, thank you once again for nice explanation.