Modify FE Mesh by Editing CAE file directly?
Modify FE Mesh by Editing CAE file directly?
(OP)
I need to do FEA on many similar organic parts. So rather than generating meshes and cae files for each of them, I would like to deform a master FE mesh to each of the parts. The deformation algorithms I have developed elsewhere, so no need for help on that.
What I am hoping for is the ability to access a list of vertices of the FE mesh through the CAE file, modify the locations, and put them back into the cae file, then run the new sim.
I tried to open the CAE file in notepad, and as I suspected, its a bunch of giberish! :-<
Anyone have any ideas how to do this?
Thanks,
Sam
What I am hoping for is the ability to access a list of vertices of the FE mesh through the CAE file, modify the locations, and put them back into the cae file, then run the new sim.
I tried to open the CAE file in notepad, and as I suspected, its a bunch of giberish! :-<
Anyone have any ideas how to do this?
Thanks,
Sam





RE: Modify FE Mesh by Editing CAE file directly?
RE: Modify FE Mesh by Editing CAE file directly?
The parts are organic and the deformations are free form, so need to have the ability to translate each FE mesh vertex independently for the part.
Could you show me a sample script for translating a FE mesh vertex, or maybe point me in the right direction?
Thanks,
Sam
RE: Modify FE Mesh by Editing CAE file directly?
Han primo incensus
RE: Modify FE Mesh by Editing CAE file directly?
Really I just need a list of FE mesh vertices for a part so that I can use my deformation algorithm to translate the vertices, then replace the original vertices in abaqus with the new vertices. It would be great if I could get the mesh vertices in a text file from abaqus, modify them, and then give the text file back to Abaqus.
I'm not even sure where the input file resides, how to get it from a cae file, and how to put it back into a cae file...
Thanks,
Sam
RE: Modify FE Mesh by Editing CAE file directly?
Your macro (or whatever it is) can then either modify it or create new ones.
HTH,
Dan
Han primo incensus
RE: Modify FE Mesh by Editing CAE file directly?
That's got me rolling for now, I may have some more questions down the road on this same topic.
Thanks again,
Sam
RE: Modify FE Mesh by Editing CAE file directly?
But I still like to look at (and work in) the deck manually. At lot of times it is more efficient and is always the end product from your pre processor.
Being familiar with a deck has many advantages. One notable one is that it is sometimes easier to communicate/demonstrate how you set up a problem since sharing a deck is easy. It is also pre/post independent (many ABAQUS users still use Patran). You can also build entire models without having to use a pre processor so it can be very efficient to run parametric studies.
Brian
www.espcomposites.com
RE: Modify FE Mesh by Editing CAE file directly?
For the original question, I presume by vertices of the mesh you mean mesh nodes? Its very easy to map mesh nodes within CAE with python...for example here's a snippet of code that maps a flat orphan mesh part onto a cylindrical one in CAE.
for eachnode in MeshPart.nodes:
theta=eachnode.coordinates[1]/Radius
newcoord1=eachnode.coordinates[0]
newcoord2=(Radius-eachnode.coordinates[2])*cos(theta)
newcoord3=(Radius-eachnode.coordinates[2])*sin(theta)
MeshPart.editNode(nodes=eachnode,coordinate1=newcoord1,coordinate2=newcoord2,
coordinate3=newcoord3)
RE: Modify FE Mesh by Editing CAE file directly?
I can't say that I've done a lot with the inp files but I've played with them now and then.
Han primo incensus
RE: Modify FE Mesh by Editing CAE file directly?
I'm calculating the deformations withing a plugin for Rhinoceros 3D, so it is really convenient to just modify the inp file as a text file and send that off to abaqus on any computer.
The models are fairly complicated and the deformations are large, so I'm hoping the FE mesh isn't distorted beyond use... If thats the case, then maybe I will use python instead, automate the remeshing and so on...
In regards to the inp file, I should probably check out the manual for a detailed guide on each line. Is that the best way to learn?
Couple quick questions I had about it:
- nodes are listed as such: number, x-coord, y-coord, z-coord
how does abaqus know which node to connect to which node to form an element? Is it just the first 4 form the first tetrahedron, the second four form the second tetrahedron (in the case of tetrahedrons?)
- picked surfaces are described by a long string of numbers, these are just referring to nodes?
Thanks!
Sam
RE: Modify FE Mesh by Editing CAE file directly?
With that said, a flattened deck will start with a node table
*NODE
Node number, x coordinate, y coordinate, z coordinate.
1, 0.0, 0.0, 0.0
The solver knows how to turn these into elements with the element connectivity table.
*ELEMENT, TYPE=...
element number, node 1, node 2, node 3, ....etc..
1, 1, 2, 3, 4...etc.
Surfaces are then defined based on the elements defined above
*SURFACE
element number, face identifier
1,S1
The manual is very good detailing what the data lines required for a given element type are.
RE: Modify FE Mesh by Editing CAE file directly?
By right clicking on the job and selecting 'write input', I get the input file. How do I get the flattened input file?
Thanks,
Sam
RE: Modify FE Mesh by Editing CAE file directly?
noPartsInputFile=ON
OR enter the following line into the small command window at the bottom of the CAE sessions
mdb.models['model name'].setValues(noPartsInputFile=ON)
Depending on which version of CAE you're using, I believe there's a check box somewhere for 'use parts and instances'. You may be abe to just uncheck it.
RE: Modify FE Mesh by Editing CAE file directly?
Cheers,
Sam