Abaqus restart analysis

[Konsti]

Hi,

Anyone here who has successfully restarted an Abaqus analysis using the .res and .prt and .odb files for a new model? Documentation, which is usually pretty good, seems overly complicated in this case and somehow missing some information (which could be "common sense", but not to me).

- Do I need to create a new model by copying the one I used to carry out the first analysis step? Or do I import the .odb file directly?
- When do I save the predefined field "initial state" and why do I always get an error that "at least one unmeshed instance has been selected..."?
- Why are BCs, loads, and connector wires not imported? That's a lot of extra work if I need to redefine them!

Thanks in advance and cheers,

Konsti

 

[FEA way]

It seems that what you mean is import analysis, this is something different than restart (there are some common features though).

In Abaqus/CAE the procedure for import is as follows:
- request restart for original analysis (Output —> Restart Requests)
- run the original job
- copy the model to new one
- define initial state field (Predefined Fields —> Initial state)
- do the necessary changes to the new model

Some features can’t be imported but it also depends on the type of import (between which solvers the results transfer is done). Other features have to be respecified.

 

[Konsti]

I actually meant the restart analysis: that is to start an analysis (explicit dynamic in my case) on an already loaded/deformed/stressed structure. It seems that Abaqus CAE has limited functionalities regarding this. I am 99% positive I heard of people simply generating a restart model without having to redefine anything..

 

[FEA way]

In the case of restart the procedure is similar with some small changes:
- request restart for original analysis (Output —> Restart Requests)
- run the original job
- copy the model to new one
- in the new model specify the restart location (Model —> Edit Attributes —> Restart)
- job for the new analysis has to be of Restart type

The restart model must be the same as the original one up to the point of restart. So you can’t modify:
- geometry, mesh and materials in general
- steps, loads, BCs, interactions, fields up to the point of restart

 

[Konsti]

Thank you, now this is some progress (no mention of copying models in the documentation)
So basically in the new model I simply add the next step(s) and given correct restart options and files from the previous job, I see that the analysis runs only the new steps starting from the previous ones.
However, what if I want to restart an Abaqus/Explicit analysis from Abaqus/Standard results? I can't add an explicit step in my copied model like you describe. I read something about predefined fields, but have no idea how to implement them.

Konsti

 

[FEA way]

If you want to change solvers (Standard instead of Explicit or vice versa) then you have to use import instead of restart. The differences between these two procedures are described at the beginning of the documentation chapter "Transferring results from one Abaqus/Standard analysis to another".

 

[Konsti]

Thank you, I seem to be getting the hang of it now.
One more question regarding the import details: I see a lot of details need to be taken care of regarding the materials, connectors, etc. In my case for example, the connector forces and displacements are *not* transferred to the new analysis by the initial state predefined field, because I can only choose part instances when I set this predefined field and not connectors. The documentation talks about importing the connectors, should that be an extra step?

 

[FEA way]

Connectors can be imported from Standard to Explicit (but not vice versa). Furthermore, when connectors are imported, you can either update reference configuration or import the state - not both at the same time.

Note that in some cases it might be necessary to use keywords for import since Abaqus/CAE has some limitations.

 

[Konsti]

Hi and thank you for the continuing help.
I don't understand the above: I have created a copy of the model, so the connectors are already there. I imported the initial state using a predefined field, but this can only be applied to meshed elements, not connectors (I can't even select them in CAE). When I run the analysis, the stresses and displacements in the elements (as well as the step number and time) continue from the previous analysis. However connectors start from zero displacement and force, which is wrong. How can I make them start from their previous force/displacement state? I don't want to update the reference configuration: I would like to simply continue deforming my model using a different solver (explicit).

Edit: diving into the documentation, I don't see an explanation of "configuration" and "state" of connectors: configuration being to which nodes they are attached to? And why not being able to import both? Do I need to *not* import the material state in order to import connector state?

Konsti

 

[FEA way]

Connectors are internally defined as elements, try importing them manually (using keywords).

Update of the reference configuration is what you can enable in Initial State field (or use Update=Yes/No parameter for keywords). By default state is always imported but you can change this with State=No parameter.

 

[Konsti]

Thank you again.
The initial state only accepts instances and not elements or sets, I could not figure out how to do it manually or using the python interpreter. Also the documentation seems very poor on how to do this, unless I am missing a specific chapter somehow.
However, looking more carefully at running an import analysis, while the instances and step number & time are clearly continuous, the loads (which I reapply instantaneously to allow for continuity) and the connector forces and displacements jump to their values from the previous analysis instantaneously in the first analysis increment. This seems correct. Therefore I do not need to do any extra imports? Simply copying the model and importing the initial state of the *instances only* is enough?

 

[FEA way]

In Abaqus/CAE the definition of import is based on instances. But if you define import manually (by editing keywords in the input file) then you can use element-based approach (import element sets). An example of this type of definition is available at the end of the documentation chapter "Transferring results between Abaqus/Explicit and Abaqus/Standard". Keywords necessary for this procedure are also separately described in Keywords Guide.

 

[Konsti]

Are you saying that using the python interpreter I cannot import connectors and the only way would be to edit the .inp file? I am scripting my model entirely and this would mean a lot of trouble: I would have to generate the model .inp file using python (without the initial state), then go into the .inp file and delete the parts and assembly and replace them with the *IMPORT and *IMPORT ELSET keywords. Or script the entire model directly in the .inp file, however I would need to learn that from the beginning (I cannot afford the time for this unfortunately).

 

[FEA way]

Several options in Abaqus are still not supported by GUI and have to be implemented using keywords. As an alternative, in many cases you can use built-in Keyword Editor but it may cause problems when the model is rebuilt. Even options not supported by Abaqus/CAE can be scripted (like pretty much everything in Abaqus) but it might be somewhat problematic. If you have access to Isight, it might be easier to automate the analyses using this software.