Learning Forum

[pierre.buchholz96]

Hello, I am an Ansys beginner and I am working on a project in which I want to simulate a multi-stage cold forming process. I am doing this in the ‘Transient Structural’ module. Unfortunately, I can't get any further with the third stage. As you can see in the first image, this step, like the other 5, consists of a PART of a DIE and a RAM. On the RAM there is a displacement (Discplacement 1 lies on the upper surface of the RAM and Dicplacement 2 serves as support) of 10.38mm which is there to press the PART into the DIE and thus reshape the PART. Unfortunately, this extrusion process of the third stage does not work, as the PART does not go all the way down. As you can see in the 2nd picture, it seems that a kind of barrier is created at the place of the taper, which prevents the PART from going any further down. I strongly suspect that this could be due to my contact conditions. The 3rd picture shows the first contact between the RAM and the PART and the 4th picture shows the contact condition between the PART and the DIE.
I would appreciate any ideas and suggestions as I am at a loss. 
Thanks in advance. 

[peteroznewman]

If the symmetry conditions include the face that is scoped in Displacement 2, then you can delete Displacement 2, but it does no harm.

In the Frictionless Contact, under Geometric Modification, Interface Treatment you have Adjust to Touch. That causes the geometry to move around in unpredictable ways at the start of each simulation. I suggest you use the setting of Add Offset, No Ramping with an offset value of 0 and do this for all 5 simulations.

[pierre.buchholz96]

Thanks for your reply. I tried to run the simulation with Add Offset, No Ramping with an offset of 0 but the part still does not go to the bottom at the die.

[peteroznewman]

Try increasing the Frictional Contact Pinball Radius to 10 mm. There is no reason to make it so small is there?

Please click the Solution Information folder and look at the Solution Output. Use Ctrl-F to search for the word error. Copy some of the text above the error into your reply.

Change from Solution Output to Newton-Raphson Force Residual plot. Take a screen snapshot and show us the progress of the solution.

If the messages show that the solution fails to converge, change the Minimimum Substeps to 200.

Make a copy of your project to try replacing Transient Structural with Static Structural analysis by a right click on the top of the analysis and use the drop down menu. See if you can get the Static Structural analysis to converge. A RAM velocity of 1.67 m/s may be slow enough that inertia forces are small enough to neglect.

[pierre.buchholz96]

 

 

 

 

it took a while to simulate this, but it was cancelled with this error: 
(I did it with minimal steps of 200 and a pinball radius of 10mm but not in static structure yet, I will try this now)

*** ERROR ***                           CP =   28162.141   TIME= 02:29:06
 An error has occurred in the Distributed Sparse Matrix Solver used by  
 the PCG solver while saving the solver workspace data.  Error code =   
 18.  Please send the data leading to this operation to your technical  
 support provider, as this will allow ANSYS, Inc to improve the         
 program.                                                               
 
 ERROR: Worker process(es) with rank(s) 2 have encountered a FATAL error.
 The information below was gathered from the file*.out output file(s).
 Please review the worker process output file(s) listed below for more
 details on this error.
 
 
 Worker Process Output File .\file2.out:
 
*** FATAL ***                           CP =   28081.828   TIME= 02:29:06
 MPI error code = 943788558 which translates to:                        
 Message truncated, error stack:                                        
 PMPI_Allreduce(388)…………………….:                          
 MPI_Allreduce(sbuf=0000006D58DEB32C, rbuf=0000006D58DF3340, count=1,   
 datatype=MPI_INT, op=MPI_MAX, comm=MPI_COMM_WORLD) failed              
 PMPI_Allreduce(374)…………………….:                          
 MPIDI_Allreduce_intra_composition_beta(775).:                          
 MPIDI_NM_mpi_allreduce(134)……………..:                          
 MPIR_Allreduce_intra_auto(60)……………:                          
 MPIR_Allreduce_intra_recursive_doubling(175):   

 

 

 

The simulation in the ‘Static Structural’ module worked! Thanks for the tip with the pinball