Importing an Orphan Mesh with a Stress Field

[aorsi]

Hello All,

I have a successful simulation with a structure which has undergone a stretch. I would like to import that part into a new model with the stress and strain still incorporated into the part, but in a new model. I am able to import the orphan mesh, but I am trying to apply a "Predefined Field" to it. I have the nodal output of stress for each node in the part. However, I do not know how to apply these nodal outputs to the orphan mesh that I have created. Is there a way to import an orphan mesh with the stress incorporated in it? Am I on the right track? Thanks a bunch!

Thanks

 

[MechIrl]

Yes you are. You'll need to use the *IMPORT keyword. This can be done through CAE by applying an 'initial state' predefined field which obtains the stress state from a previous analysis job.

 

[aorsi]

OK,

I understand what you are saying. I am running into a problem when I type the Job Name of the previous analysis job, it says it cannot find the .res file. I am wondering what this means. I have tried to find a .red file in my working directory, as well as my temp folder, and have nothing. Any help would be greatly appreciated.

Thanks,

-Alex

 

[MechIrl]

The RES file is one of several files you need to restart an analysis. If you are running an Abaqus/Standard analysis its probably not created by default. You'll need to specify how many times you want restart data written before you run the analysis using the *restart keyword or from within CAE in the step module. If you are running an Abaqus/Explicit analysis you should have a RES file already if the job comleted successfully.

 

[aorsi]

So I have been reading the manual. I am wondering if what I want to do is impossible. I have 4 parts that I have performed a displacement to, creating a stress field in the mesh of these parts. I would like to import these 4 parts into a new assembly, with the stress fields attached. But apparently, the *INITIAL CONDITIONS does not work for an assembly. is this correct? I also am unsure how to use the *IMPORT command. is this different than the *INITIAL CONDITIONS command? any help would be greatly appreciated.

Thanks

 

[aorsi]

Ok,

So the reason I am trying to do this procedure is because I am running an extension test, which is to be followed by a rotation. Imagine a cylinder that is stretched to a solid body. then, that solid body rotates. But when the solid body rotates, the cylinder needs to rotate with the solid body. I am trying to extend the cylinder structure to the solid body. Then have it mate at that time. THEN, i want to rotate the solid structure. But I cannot find out a way to apply a step specific tie constraint, or a couple constraint. This is why I am trying to run the extension test, then export the mesh with the stress, and then run the rotation step. If you have any input on how I should model this or other ways rather than trying to model this extension, then rotation, I would really appreciate it.

Thanks,

-Alex

 

[MechIrl]

Yes I think using the import approach will be a good way to model this, as it allows you to implement the tie contraint after the fist analysis. As far as I'm aware the *initial conditions keyword cannot be used for this kind of thing. The *import command is different however, you should be able to use it on whole assemblies. I often use on multiple part assemblies after large deformation analyses and it works well.

The easiest approach to this is through CAE, hopefully you have access to it! The approach I use is to import the INP file from the original analysis, then assign predefined fields to each part in the assembly using the initial state option. After this you can implement the new tie constraints, even if the surfaces are not in contact in the original configuration.

There are probably other ways to approach this but I think using an import analysis is a fairly streight-forward way to do it.

 

[aorsi]

Hello,

Thanks for responding, I really appreciate the feedback. I am still running into the same problems with your method. However, I am able to import the deformed mesh into my new assembly. But I have the following problems.

1) I tried importing the INP file as you had said...But this does not provide the deformed geometry that I need...Why would I import the INP file from the initial simulation? is there something important from this file that I need to use?

2) The predefined field option is still giving me the .RES file error. I went into the step menu as you had suggested, and do not understand how to tell abaqus to create this file.

any help would be greatly appreciated.

this seems like such a basic thing...I really cannot believe I am having trouble with this. But again, thanks for all the help!!!!

Thanks,

-Alex

 

[MechIrl]

Ok, so for point 1. No it isn't a neccesity to import the input file to do an import analysis. I just find it a convenient way to perform it, as it means I have access to all the set definitions for that particular model, bearing in mind that its necessary to redefine any constraints from the pevious analysis. You don't need to have the deformed part geometry to do the import analysis, which seems weird at first, but essentially abaqus generates the deformed shapes automatically based on information (essentially nodal displacements) stored in the RES file.

For point 2. You tell abaqus to generate restart data in the step module by going to Output>Restart Requests and changing the number of intervals to the number of times restart data will be requested in the analysis.

Hopefully this helps...

 

[aorsi]

Hi MechIrl,

I cannot thank you enough. You have been a great Help. So i have successfully imported the predefined field. However, I am now receiving errors based on my surface ties. It doesnt like the surface tie selections I have given it...this seems odd. I was wondering if you have any input on this, or if there are special ways to define the surface interactions with an imported orphan mesh.

Thanks,

-Alex

 

[aorsi]

For some reason, I am recieving these errors when I try to run a simulation after I import the orphan mesh.

------------------
This option is not supported for element loop parallelization. If you have specified element loop parallelization, it will be turned off for this analysis.

Material/behavior placl has been redefined in the current analysis. Care must be taken to ensure that a consistent state can be maintained during the import procedure.

For *tie pair (assembly__pickedsurf98-assembly_femur-1_acl_insert), not all the nodes that have been adjusted were printed. Specify *preprint,model=yes for complete printout.

For *tie pair (assembly__pickedsurf98-assembly_femur-1_acl_insert), adjusted nodes with very small adjustments were not printed. Specify *preprint,model=yes for complete printout.

The system matrix has 23196 negative eigenvalues.

Excessive distortion at a total of 19291 integration points in solid (continuum) elements

--------------

the negative eigen values stay the same for a few iterations, and the excessive distortion reduces for each iteration. However, the final error is that too many increments are made for this increment. so I am unsure why this is happening.

Thanks,

-Alex

 

[MechIrl]

Without seeing the problem itself its a bit difficult to say what might be going wrong. Are you importing the deformed orphan mesh geometry for the import analysis or undeformed? I think both should work but it may be more appropriate to work with the undeformed geometry, it makes it easier to introduce the correct tie constraints.

Did the analysis produce any output? If you can see the analysis results then maybe you'll get an idea of which elements are most distorted?