Boundary Conditions on Deformed Configuration

[FBMeca]

Hello there!

I'm modeling a forming process in which I have the following :
- A first step in which the forming tool performs a first deformation of the metal sheet. I have used displacement boundary conditions (BC's) to model this (e.g. z-displacement of 10mm, encastre BC's, etc.)
- I want to include a second step, with different boundary conditions for the tools, in which the forming tool would then perform another z-displacement of 5mm for example. From what I know, displacement BC's are always defined to the reference/initial configuration, and not to the deformed configuration of step-1 (which is what I want).

My questions :
- Are there other possibilities to simulate this 2-step forming process? I have seen I can simply use velocity BC's for displacement boundary conditions, but would this also apply to displacement BC's where I constrain some displacement (rotations for example to avoid rigid body motion which would then become zero velocity for these rotations)?
- Is an ENCASTRE BC also related to the initial configuration? How to apply an ENCASTRE BC on the deformed configuration (after step-1)?
- Would it be better to simply define the deformed configuration after step-1 as the new initial configuration for step-2? If so, how to do this?

Thanks a lot for your help!

Fernand

 

[FEA way]

Such forming processes with multiple stages are often simulated using the import functionality in Abaqus. It’s described in the "Importing and transferring results" documentation section. Basically, it allows you to import the deformed shape and material state from one analysis to another in which different boundary conditiona, loads and other features are defined.

 

[FBMeca]

Hi FEA way,

Thanks for your response. I had indeed missed that. I read it throught but am still a bit confused :
- When choosing Predefined field > Other > Field, do I then need to choose "From results or output database file"? So this means I need to simply run a first job with the model containing step-1 only, and have this as an input to the second model with step-2 only?
Or is there a way for Abaqus to do it automatically by itself and have both steps in one model and run the job once only?

Thanks!

 

[FEA way]

With this procedure there are 2 separate analyses. For the second one you have to specify the deformed mesh and materual state from the first one plus define new steps and their features. Of course, this can be automated using scripting. Another option is restart functionality but it’s just multistep analysis split into more than one run.

 

[FBMeca]

Alright, perfect!
What I did was simply importing all the parts from the .odb of step-1 simulation, and then create these instances in the assembly module.
But will there not be any difficulties for Abaqus at the beginning of the simulation to initiate the contact analysis since everything is already in contact so to say?

Also, when creating a predefined field with the initial state, it tells me it also needs the restart .res file. Why is this the case? Does this simply mean I need to also add the .res file of the last increment of my step-1 simulation?

Thanks!

 

[FEA way]

When working with Abaqus/CAE, this functionality is usually used by copying the original model and preparing import analysis in the copy (deleting unnecessary parts, defining the initial state field and so on). What can and what can’t be imported depends on the solvers - if it’s Standard <—> Explicit or Explicit —> Explicit.

Indeed, the restart data from the original analysis is necessary for this procedure (and for the restart procedure described above, of course) so you have to request it for the first stage.

 

[FBMeca]

Alright, thank you!
When running my step-2 simulation, it returns me an error saying it needs a .mdl file.
I don't really know how to generate this model file (which I don't get by default when running my .inp), could you help me on that?

Also, I'm still confused why use the term "restart". I'm just running a full simulation on my step-2 model and am not doing a restart of the previous simulation, is that correct?

Thanks a lot for your help.

 

[FEA way]

If you add a restart request to the first analysis (using Abaqus/CAE or keywords directly), you should get all the necessary files for the second analysis. Restart data is just needed for both functionalities - restart and import, even though they are used for different purposes (but are both analysis continuation techniques).

 

[FBMeca]

I have indeed found the .mdl file by now, I wasn't looking well enough..

Another question I'd have is that when I import all the deformed parts of the stage-1 simulation, old sets appear with different namings as well as new sets that I had not defined in the stage-1 model. Can I delete all the sets and surfaces and create new ones, or should I retain the ones after doing the import? Concerning their naming, it's also not a problem if these different sets + surfaces have different names in stage-2 compared to stage-1?

But I guess the only thing that is important is to keep the name of the parts identical (in step-2 compared to step-1) when importing them?

Fernand

 

[FEA way]

Keep the sets that you need for definitions of features in the second analysis, removing the rest shouldn't cause any problems. Like I said before, when working with Abaqus/CAE the best way to use the import technique is to copy the original model. Then you can just remove the unnecessary instances, features and sets and keep the ones that are needed for the second analysis. Only the initial state field connects the new analysis to the previous one. The rest forms new definitions in the second analysis.

 

[FBMeca]

Alright, now it's clear, thanks!

I've been doing what you told me to do, ran the input file for the step-2 simulation, but the Analysis Input File Processor exits with an error (pasted relevant lines only):

***ERROR: The surface ASSEMBLY_SHEET_SHELL-1_CONZMAX has not been defined.
LINE IMAGE: ASSEMBLY_DIE-1_CONTACT, ASSEMBLY_SHEET_SHELL-1_CONZMAX
***NOTE: DUE TO AN INPUT ERROR THE ANALYSIS PRE-PROCESSOR HAS BEEN UNABLE TO
INTERPRET SOME DATA. SUBSEQUENT ERRORS MAY BE CAUSED BY THIS OMISSION

***ERROR: The surface ASSEMBLY_SHEET_SHELL-1_CONZMAX has not been defined.
LINE IMAGE: "ASSEMBLY_Outside die-1_CONTACT", ASSEMBLY_SHEET_SHELL-1_CONZMAX

***ERROR: The surface ASSEMBLY_SHEET_SHELL-1_CONZMIN has not been defined.
LINE IMAGE: ASSEMBLY_PUNCH-1_CONTACT, ASSEMBLY_SHEET_SHELL-1_CONZMIN

***ERROR: The surface ASSEMBLY_SHEET_SHELL-1_CONZMIN has not been defined.
LINE IMAGE: "ASSEMBLY_Outside punch-1_CONTACT", ASSEMBLY_SHEET_SHELL-1_CONZMIN

***ERROR: The surface ASSEMBLY_SHEET_SHELL-1_CONZMIN has not been defined.
LINE IMAGE: ASSEMBLY_HOLDER-1_CONTACT, ASSEMBLY_SHEET_SHELL-1_CONZMIN
*contactpropertyassignment

***ERROR: *CONTACT INCLUSIONS suboption is required for defining the general
contact domain.

Apparently, there is some problem with the surfaces. I defined two surfaces ConZMAX and ConZMIN (which are shell surfaces) in the new assembly, and am using General Contact by including surface pairs. I tried deleting the surfaces and creating them again but the same error appears again..

Would you know what this could be due to?
Many thanks.

 

[FEA way]

Those errors occur for the approach in which you import the deformed mesh from odb, right ? Try the one with copying the original model or prepare the input file manually if you are familiar with keywords (you just need a blank input file with *IMPORT and keywords defining the second analysis). The template can be found in the documentation.

 

[FBMeca]

Yes exactly, this occurs when importing the deformed mesh from .odb.

I found the template you mentioned, I will try look into it. So there can be issues when using this import from .odb option which can be avoided with this *import keyword?
As for your other suggestion, what do you exactly mean with "copying the original model"? I don't see the point of this since when copying the model of the step-1 simulation, I would also need to import the new deformed parts in some way (which comes down to what I did up to now?) ?

 

[FEA way]

The easiest way is to:
1. Copy the original model into a new one
2. Delete unnecessary instances, sets, boundary conditions and other features, keeping only the ones relevant in the second analysis
3. Define the initial state field
4. Define new analysis features

That's it, no need to import the deformed mesh with this approach. Step 3 will account for that.

 

[FBMeca]

Okay now I totally get it. I thought importing deformed parts was needed..
But is it then correct that I need to tick the "Update reference configuration" when creating Predefined-field > Initial state ? If not, how does abaqus know that displacement BC's are now defined with respect to the final configuration of the Step-1 simulation?

Thanks!

 

[FEA way]

Updating reference configuration means that displacements and strains will be reset to zero for the second analysis. This is used for springback simulations. Not updating it means that displacements and strains will be continued from the first analysis. This is used for multi-stage forming simulations.

 

[FBMeca]

Okay, but then, in my simulation of Step-2, will it automatically take the displacement boundary conditions of the tools (e.g. 10mm z-displacement of tool A...) with respect to the deformed configuration at the end of Step-1?

EDIT : I followed the 4 steps you mentioned, and obtain the same error as before. So when generating the .inp file, I see that indeed the *Elset and *Surface definitions are now missing when adding this predefined field. Is this normal? Therefore, Abaqus just gives me the error that it cannot find these surfaces because they are not defined in the .inp of the Step-2 simulation...

 

[FBMeca]

I will try to sort this out myself as these issues seem to come from the fact that I called my parts with two words in the simulation of stage-1 such as "Tool One" which seemed to be problematic..

If you could just help me on these two last questions, I'd be grateful :

- As far as the more straightforward modeling is concerned, by just defining two steps in one simulation, I have seen I can simply use velocity BC's for displacement boundary conditions. Would this also apply to displacement BC's where I constrain some displacement (rotations for example to avoid rigid body motion which would then become zero velocity for these rotations)?
- Is an ENCASTRE BC also related to the initial configuration? How to apply an ENCASTRE BC on step-2 but if I want to fix one of the tools in the deformed configuration (after step-1)?

Again, thanks a lot for your time.

 

[FEA way]

Yes, you can use zero velocity boundary conditions instead of zero displacement ones. In fact, this approach is recommended for Abaqus/Explicit analyses.

Boundary conditions applied in the second analysis will work on the imported (deformed) configuration of the model.