How to do spring back analysis in Abaqus 6.7

[B1ackMi16]

Hi!

I'm trying to do spring back analysis on a tube that I bend using Abaqus Explicit.

I have tried just to make the bending mandrel bend the tube to 50 degrees, and then take it back to zero degrees, but the profile will then start oscillating.

What I need to do is to get the stresses from the last timestep in the explicit analysis, and use this as input stresses for a standard implicit analysis.

Anyone got any tips/hints?

Regards

Kristian

 

[bassmanjax]

There's an example problem in the docs - see "1.5.1 Springback of two-dimensional draw bending". This more or less covers what you need to know.

Regards

Martin Stokes CEng MIMechE

 

[B1ackMi16]

Thanks for your help! This is almost exactly the same thing I need to do.

However I still have some problems.

I took the input file with the IMPORT command from the example and tried to use it on my own analysis.

However when I try to import this file into Abaqus CAE it will open as a new model and give this message:

"The model "boyetest_statisk_import" has been created.
WARNING: Empty part PART-1. This occurred while reading keyword options within part definition.
WARNING: Part instance PART-1-1 references an empty part. A new part named PART-1-1 will be created from the mesh data in part instance PART-1-1.
WARNING: Empty part instance PART-1-1. This occurred while processing part PART-1. Neither the original part nor the part instance PART-1-1 contain mesh data.
"

I was thinking I should get this as an additional step inside the original model.

I've also tried just to make a new step in the original model, but it will only allow me to make Explicit Dynamic steps and not Standard Static as I need.

Regards

Kristian

 

[bassmanjax]

I don't use CAE for pre-processing, so I've just had a scan through the manuals.

Section 16.6 covers the transfer of results between Explicit and Standard. Might be worth your while to have a read through that first.

To be honest, the input deck for a springback analysis will be quite small. All you need to do is add the *INSTANCE and *IMPORT for each part you need. The *STEP required will be just a single *STATIC step. The only trick is to make sure that the model is sufficiently constrained to prevent any rigid body motions.

See the attached file for a fairly typical springback that I did on a previous Explicit forming step.

I've also tried just to make a new step in the original model, but it will only allow me to make Explicit Dynamic steps and not Standard Static as I need.

You can't mix Standard and Explicit steps in a single analysis - that's why you need the *IMPORT functionality.

Regards

Martin Stokes CEng MIMechE

 

[B1ackMi16]

Again thanks for your help Martin!

I've been looking some more into the input files, both my own and yours to try to figure out how to use this.

Am I right I need to run the spring-back analysis from the command prompt, "abaqus job=springback" if I call the new input file springback.inp?

I have attached my input file for the first (Explicit) part of the analysis and this runs fine and bends the tube.

Then I have now used your input file for springback which I have modified to this:

-------------------------------
**
** Decatur die necking
** Stage 1 springback
**
*assembly, name=Springback
**
*instance, instance=FE_MODEL, library=boyetest4_2_cae
*import, update=yes
**
**
*end instance
**
*end assembly
**
*Boundary
BC_BAKKANT, 1, 1
BC_BAKKANT, 2, 2
BC_BAKKANT, 3, 3
BC_BAKKANT, 4, 4
BC_BAKKANT, 5, 5
BC_BAKKANT, 6, 6
**
*step, nlgeom
Die Necking Stage 1 Springback
*static
0.01,1.0
**
*output, field, variable=preselect
**
*output, history, variable=preselect
**
*restart, write
**
*end step
**
-------------------------------

Am I right that the IMPORT function will import all the node- and element sets from the first analysis, so I can directly refer to those when setting the boundary conditions as I have done here?

The spring back analysis still doesn't work, so I guess there are something wrong in the code above. I'm really new to this way of working with a FE system, have mostly used GUI systems before.

Also when using the IMPORT as it is done in this case, I guess it will import the whole model geometry and not only the tube which is what I really wanna look at.

I guess I have to use the *IMPORT ELSET and/or *IMPORT NSET function but find the lack of examples in the documentation kind of hard, as is's not easy to get it how to use the different parameters properly. I only want to import the elements and nodes. The elements of the tube are defined by element set NX_2D_MESH(1), and it's nodes from node set ROR. The only boundary conditions that shall apply are all six degrees of freedom is locked on node set BC_BAKKANT.

Again thanks for your help, and I understand if I'm asking a bit too much now, but I'm quite stuck with this.

Regards

Kristian

 

[bassmanjax]

The node and element sets should come in okay. What is the error message when you try to run the job?

Having looked at your original input deck, you will need to change the following in the springback analysis;

- The assembly name must be the same for both input files. In your explicit deck it is NAME=Assembly and in the springback analysis, NAME=Springback - this won't work. Make it NAME=Assembly.

- I didn't have any contact in my input file. If you have any in yours, you will need to add in the required *CONTACT PAIRS. Remember that general contact is not available in Standard!

And yes, you will have to run the job from the command prompt.

Regards

Martin Stokes CEng MIMechE

 

[B1ackMi16]

Thanks again, I got some errormessages that I found in the .dat file.

I have now removed initial temperature from input file, and made the materials more simple not temp. dependent as the springback.inp analysis wouldn't work with the init temp setting.

I can now open the Springback.odb file into CAE and I will see the deformed geometry from last step in the explicit analysis. Which is a good step in the right direction

The analysis will run if I don't set any BC's, but it will of course not converge so it exits with error.

When I try to set BC's I also get this message in the .dat file:
***ERROR: in keyword *BOUNDARY, file "Springback.inp", line 15: Unknown
assembly node set BC_BAKKANT
***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

Later on I also get these errors:
***ERROR: NODE SET "ASSEMBLY_BC_BAKKANT" HAS NOT BEEN DEFINED
***ERROR: A BOUNDARY CONDITION HAS BEEN SPECIFIED ON NODE SET
"ASSEMBLY_BC_BAKKANT" BUT THIS NODE SET IS NOT ACTIVE IN THE MODEL

The IMPORT command also seem to import the whole geometry. I've tried to make it import only the elements I want with putting the *IMPORT ELSET command after the import, but did not seem to work either.

Quite a few things wrong still

 

[bassmanjax]

To correct the nset error, you need to use the correct terminology, i.e. instance.setname, so;

In your *IMPORT statement, the instance name is;

*instance, instance=FE_MODEL, library=boyetest4_2_cae

so,

*boundary
BC_BAKKANT
...etc

should be;

*boundary
FE_MODEL.BC_BAKKANT
...etc

You must reference the instance if it is an instance level node set. You are trying to reference a non-existant assembly level node set, hence the error.

Regards

Martin Stokes CEng MIMechE

 

[B1ackMi16]

Thanks again Martin.

I've now managed to run the spring back analysis

I had to change my first analysis file and separate the mesh into two parts one for tool and one for tube/blank.

This way I was able to just import the tube instance when doing spring back analysis.

However I was still not able to use the nodeset BC_BAKKANT for setting the boundary conditions in the new input file, so I had to manually define this nodeset again in the springback input file. After I did this the analysis did run fine

When I refer to the existing nodeset in the BC (ROR1.BC_BAKKANT) I get this message (The instance name of the tube is now ROR1):

***ERROR: in keyword *BOUNDARY, file "Springback3.inp", line 391: Unknown part
instance node set ROR1.BC_BAKKANT

Further down I also get this:
***ERROR: NODE SET ASSEMBLY_ROR1_BC_BAKKANT HAS NOT BEEN DEFINED

I guess this must be due to a small issue in my code.

*HEADING
** Spring back analysis of tube
*ASSEMBLY, NAME=Assembly
*INSTANCE, INSTANCE=ROR1, LIBRARY=boyetest4_4_cae
*IMPORT, STATE=YES, UPDATE=YES
NX_2D_MESH(1)
*END INSTANCE
*END ASSEMBLY
**
*BOUNDARY
ROR1.BC_BAKKANT, 1, 1
ROR1.BC_BAKKANT, 2, 2
ROR1.BC_BAKKANT, 3, 3
ROR1.BC_BAKKANT, 4, 4
ROR1.BC_BAKKANT, 5, 5
ROR1.BC_BAKKANT, 6, 6
**
*RESTART, WRITE
*STEP, nlgeom
SPRINGBACK
*Static
0.05,3.0
*OUTPUT, FIELD, VARIABLE=preselect
*OUTPUT, HISTORY, VARIABLE=preselect
*END STEP

Thanks for any help and merry christmas

Regards

Kristian