Error Message: Node set has not been defined. 1

[Varved]

I'm modeling a simple system of two layers (pavement on soil) using CAE. I'm receiving an error message similar to the one mentioned in the following thread:

thread799-186602

It reads:

Error in job matchup-elastic: NODE SET "ASSEMBLY_MESH PART-1_MESH PART-REFPT_" HAS NOT BEEN DEFINED

I'm attaching the .inp file. What needs to be defined that isn't included?

 

[vumat721]

It's unclear why you need a reference node for the type of element and section you are using. I would recommend just deleting:

, ref node="Mesh Part-RefPt_"

from both of your section definitions in the input file. Or in CAE, create new Sections in the Section Manager, make them Solid,Homogeneous type. Then, in the Section Assignment Manager, change your assigned sections to the newly created ones.

 

[Varved]

Ok, I'll try and change the section type to see what happens, but I'd ultimately like the analysis to be plane strain. After my effort, I'll post an updated file where I use the new section type and geometry definitions to place loads and bc's rather than a mesh part.

Thank for the advice!

 

[vumat721]

You can only use a Generalized Plane Strain section when you are using a Generalized Plane Strain element (e.g. CPEG4R, note the "G"). For regular plane strain (e.g. CPE4R) and every other type of solid continuum element, you just need to use a Homogeneous Section and therefore don't require a reference node.

I'm guessing you don't need the Generalize Plane Strain elements because they are for very special modeling situations. But you can learn more about them in section 22.1.2 of the Abaqus 6.8 Analysis Manual. If you do need a generalized plane strain element, then you need to create a reference node for your part in the Part module (menu Tools --> Reference Point).

 

[Varved]

Thanks vumat,
I found that to be the case, I used a homogeneous section and the analysis ran. Thanks for the help! I'm posting the file that ran in case anyone would find it useful.

Evan