On Creating Node & Element Sets

[CSAPL]

I mesh my model and now i want to apply Initial Conditions
that should be applied on ELEMENT and NODE sets
However, I tried to creat Node Set or ELement Set but I found the following choices : ALL, Vertices, Edges, Faces, Cells, Skin, Referenc Points.
No Element or Nodes . Should one transfer the mesh to an orphan mesh in order to be able to creat Element or Node Set.
Thanks for your time

 

[corus]

Assigning the geometry to a set will assign the nodes or elements associated with that geometry to that set. If it's a particular region of a part that is to be included in a set then partition that region.

corus

 

[CSAPL]

Some Initial Conditions (e.g. Void Ratio) can only be assigned to Nodes Set while others(e.g. Stress) can only be assigned on Elements Set. So if I Creat geomtry set and name it :FOUND
this can be used for both Initial Conditions descriptions:
Intitail Conditions, Type =Ratio
FOUND,............
Initial Conditions, Type=Stress
FOUND,.................

Thanks

 

[CSAPL]

COURSE I THINK YOU ARE NOT RIGHT . HER IS WHAT I GOT FROM abaqus doc QUOTE:
"Node and element sets contain nodes and elements that you have selected from an orphan mesh part. Sets that you create using the Set toolset can include either nodes or elements but not both. However, a set imported from an output database or from an input file can contain a mixture of both nodes and elements if the input file includes a node set and an element set with the same name. Although you can create node and element sets from orphan meshes, you cannot create them from a native ABAQUS part that you have meshed in the Mesh module"
I BELEIVE THAT I SHOULD TRANSFER MY MESH TO AN ORPHAN ONE IN ORDEER TO BE ABLE TO CREAT ELEMENT OR NODE SETS. DO YOU AGREE..?

 

[corus]

Try creating a set from the gemoetry and write out the input file. Look in there to see if the set has been defined in terms of nodes and elements.

Please don't use capital letters as this is inferred as shouting. People who shout the loudest may be heard but will be listened to in silence.

corus

 

[brep]

CSAPL,
We hear you loud and clear but unfortunately you are wrong. Please do as Corus and I have previously (in this thread and another), then look at the input files and get back to us...

 

[CSAPL]

Hi Brep and Corus
I will try what you've said when I get to me desk and access ABAQUS. You ,guys, would be correct as I am thinking now that the message which I got Regarding " unrecognising node set" could be due to introducing Initial Conditions (void ratio)in the Geostatic Step which I do not think should have been done. As Geostatic Step can only accommodate Initial Stress as an Initial Conditions.

BTW this is the first time where I know that capital letters could imply shouting.(Just being disorganized in dealing with the Keyboard) Forgive me for being loud. I just realized that in the past I unknowingly shouted at many people (including my managers and supervisors)

 

[gurmeet2003]

CSAPL,
I have had similar experience to you. When I have to access node/element sets I typically convert my part to an orphan mesh part. If there is any way around it I would also be curious to know.
Thanks,
Gurmeet

 

[xerf]

You can partition a part (-instance) to include the region of interest. Further, you can create a set based on that partition. You can partition volumes, faces and edges.

The advantage of defining sets based on geometric entities is that if you decide to remesh your model you do not need to recreate the nodes and element sets.

 

[CSAPL]

I created set on part and call it FOUND. I went to the inp.file I found
*Nset, Found
*Eset, Found
So it seems that creating the set in part (or assembly) will accomodate both nodes and (not or (as Corus said above)) element am I right. Let us put it this way:
Some Initial Conditions (e.g. Void Ratio) can only be assigned to Nodes Set while others(e.g. Stress) can only be assigned on Elements Set. So if I Creat geomtry set and name it :FOUND
this can be used for both Initial Conditions descriptions:
Intitail Conditions, Type =Ratio
FOUND,............
Initial Conditions, Type=Stress
FOUND,.................
Please confirm . is that right.?

 

[xerf]

The geometric and element/node sets are explained in ABAQUS/CAE User's Manual -> 48.2 Understanding sets and surfaces

 

[CSAPL]

Well I red the stuff . It it were clear enough I would not have wasted additional time the last couple of days about it. For example, Quote from manuel "Sets that you create using the Set toolset can include either nodes or elements" but when I created set on part ( call it Found). I went to the inp.file to see if Found was included as Nset or Eset but I found both :
*Nset, Found
*Eset, Found
How that discrepancy (at least for me) could be explained

 

[xerf]

If you create a part in CAE using geometric modeling then you can create geometric sets containing geometric entities. After the geometric entities are meshed, ABAQUS creates sets of elements and nodes from the elements and nodes associated with the geometric entities you included in the geometric set.