Learning Forum

[ashish35]

Hello,

I am trying to predict distortion and residual stresses in a part in ANSYS Mechanical 19.1 using the additive wizard. The simulation process perfectly converges until the step of base plate removal is reached. I know the build has to be constrained properly to get the deformation and stress state effect after the print is removed from the base, for which the three nodes I chose were 3 corners of the build which in my opinion should perfectly constrain the model in 3 translation and 3  rotational degrees of freedom, but the solution is always interrupted because of rigid body motion. Could I be given any tutorials on how to constrain the build after its removal from base. 

I have attached the model image along with this message.

Best Regards,

Ashish

[Sandeep Medikonda]

Ashish,

  Can you post some images on how you are constraining your model, the error message, and your structure tree? 

Regards,

Sandeep

[ashish35]

Hello Sandeep,

Please note that

a) node 1 is constrained in translational x,y and z,

b) node 2 in y and z 

c) and node 3 is constrained in only z

I have posted the images of tree, error message and the constraints.

Best,

Ashish

 

[ashish35]

Sandeep,

Sorry the error message is not clearly visible and the axes in model are not clearly visible. Here's a better picture of model with axes and the error message:

Best,

Ashish

[Sandeep Medikonda]

Ashish,

  I noticed that you are using APDL commands, In 19.1 you would have to set the following in Solver Process Settings:

Can you confirm if you are doing this? Also, are you using the worksheet to remove the base removal?

If none of these suggestions help can you try selecting a different node instead of the one at the very corner to constrain your model? Please select a different node which is not at the interface?

Lastly, if nothing helps, can you post the last part of your solution output using the Preformatted text option in your reply?

Regards,

Sandeep

 

[ashish35]

Sandeep,

I tried using the argument -amfg and I got this error instead:

I also selected a node which was not at the interface to constrain the model but it still didn't work:

Yes, I am using the worksheet to setup the additive process:

The solution information for the last part of my solution is as follows:

 

 

A D D I T I V E   S T E P

   STEP TYPE . . . . . . . . . . . . . . . . . . .REMOVE
   LOAD STEP . . . . . . . . . . . . . . . . . . .    30
   SUPPORT TO REMOVE . . . . . . . . . . . . . . .PLATE

     FORCE CONVERGENCE VALUE  =   3554.      CRITERION=  0.5102E-04

 *** WARNING ***                         CP =     569.906   TIME= 181:05
 The PCG solver detects that the stiffness matrix is ill-conditioned.   
 The solution has not converged.  Please check for rigid body motions   
 in your model.                                                         
                                                                        

 *** ERROR ***                           CP =     569.906   TIME= 181:05
 Preconditioned conjugate gradient solver error level 1.  Please check  
 for an insufficiently constrained model.  Switching to the sparse      
 direct solver may allow this nonlinear analysis to continue beyond     
 this point.                                                            
    >>> NEGATIVE PIVOT ENCOUNTERED
 *** LOAD STEP    30   SUBSTEP     1  NOT COMPLETED.  CUM ITER =    181
 *** BEGIN BISECTION NUMBER   1    NEW TIME INCREMENT=   401.86   

     FORCE CONVERGENCE VALUE  =   6705.      CRITERION=   28.30   
    >>> Thermal expansion factor =  0.100000   

 *** WARNING ***                         CP =     583.172   TIME= 181:18
 The PCG solver detects that the stiffness matrix is ill-conditioned.   
 The solution has not converged.  Please check for rigid body motions   
 in your model.                                                         
                                                                        

 *** ERROR ***                           CP =     583.172   TIME= 181:18
 Preconditioned conjugate gradient solver error level 1.  Please check  
 for an insufficiently constrained model.  Switching to the sparse      
 direct solver may allow this nonlinear analysis to continue beyond     
 this point.                                                            
    >>> NEGATIVE PIVOT ENCOUNTERED
 *** LOAD STEP    30   SUBSTEP     1  NOT COMPLETED.  CUM ITER =    182
 *** BEGIN BISECTION NUMBER   2    NEW TIME INCREMENT=   200.93   

     FORCE CONVERGENCE VALUE  =   3630.      CRITERION=   3.113   
    >>> Thermal expansion factor =  1.000000E-02

 *** WARNING ***                         CP =     598.719   TIME= 1814
 The PCG solver detects that the stiffness matrix is ill-conditioned.   
 The solution has not converged.  Please check for rigid body motions   
 in your model.                                                         
                                                                        

 *** ERROR ***                           CP =     598.719   TIME= 1814
 Preconditioned conjugate gradient solver error level 1.  Please check  
 for an insufficiently constrained model.  Switching to the sparse      
 direct solver may allow this nonlinear analysis to continue beyond     
 this point.                                                            
    >>> NEGATIVE PIVOT ENCOUNTERED
 *** LOAD STEP    30   SUBSTEP     1  NOT COMPLETED.  CUM ITER =    183
 *** BEGIN BISECTION NUMBER   3    NEW TIME INCREMENT=   100.47   

     FORCE CONVERGENCE VALUE  =   3557.      CRITERION=  0.3142   
    >>> Thermal expansion factor =  1.000000E-03

 *** WARNING ***                         CP =     627.156   TIME= 182:03
 The PCG solver detects that the stiffness matrix is ill-conditioned.   
 The solution has not converged.  Please check for rigid body motions   
 in your model.                                                         
                                                                        

 *** ERROR ***                           CP =     627.156   TIME= 182:03
 Preconditioned conjugate gradient solver error level 1.  Please check  
 for an insufficiently constrained model.  Switching to the sparse      
 direct solver may allow this nonlinear analysis to continue beyond     
 this point.                                                            
    >>> NEGATIVE PIVOT ENCOUNTERED
 *** LOAD STEP    30   SUBSTEP     1  NOT COMPLETED.  CUM ITER =    184
 *** BEGIN BISECTION NUMBER   4    NEW TIME INCREMENT=   50.233   

     FORCE CONVERGENCE VALUE  =   3555.      CRITERION=  0.3145E-01
    >>> Thermal expansion factor =  1.000000E-04

 *** ERROR ***                           CP =     642.734   TIME= 182:20
 Preconditioned conjugate gradient solver error level 1.  Please check  
 for an insufficiently constrained model.  Switching to the sparse      
 direct solver may allow this nonlinear analysis to continue beyond     
 this point.                                                            
    >>> NEGATIVE PIVOT ENCOUNTERED
 *** LOAD STEP    30   SUBSTEP     1  NOT COMPLETED.  CUM ITER =    185
 *** BEGIN BISECTION NUMBER   5    NEW TIME INCREMENT=   25.117   

     FORCE CONVERGENCE VALUE  =   3554.      CRITERION=  0.3145E-02
    >>> Thermal expansion factor =  1.000000E-05

 *** WARNING ***                         CP =     663.688   TIME= 182:41
 The PCG solver detects that the stiffness matrix is ill-conditioned.   
 The solution has not converged.  Please check for rigid body motions   
 in your model.                                                         
                                                                        

 *** ERROR ***                           CP =     663.688   TIME= 182:41
 Preconditioned conjugate gradient solver error level 1.  Please check  
 for an insufficiently constrained model.  Switching to the sparse      
 direct solver may allow this nonlinear analysis to continue beyond     
 this point.                                                            
    >>> NEGATIVE PIVOT ENCOUNTERED
 *** LOAD STEP    30   SUBSTEP     1  NOT COMPLETED.  CUM ITER =    186
 *** BEGIN BISECTION NUMBER   6    NEW TIME INCREMENT=   12.558   

     FORCE CONVERGENCE VALUE  =   3554.      CRITERION=  0.3145E-03
    >>> Thermal expansion factor =  1.000000E-06

 *** WARNING ***                         CP =     687.703   TIME= 183:06
 The PCG solver detects that the stiffness matrix is ill-conditioned.   
 The solution has not converged.  Please check for rigid body motions   
 in your model.                                                         
                                                                        

 *** ERROR ***                           CP =     687.703   TIME= 183:06
 Preconditioned conjugate gradient solver error level 1.  Please check  
 for an insufficiently constrained model.  Switching to the sparse      
 direct solver may allow this nonlinear analysis to continue beyond     
 this point.                                                            
    >>> NEGATIVE PIVOT ENCOUNTERED
 *** LOAD STEP    30   SUBSTEP     1  NOT COMPLETED.  CUM ITER =    187
 *** BEGIN BISECTION NUMBER   7    NEW TIME INCREMENT=   6.2791   

     FORCE CONVERGENCE VALUE  =   3554.      CRITERION=  0.5102E-04
    >>> Thermal expansion factor =  1.000000E-07

 *** WARNING ***                         CP =     710.625   TIME= 183:29
 The PCG solver detects that the stiffness matrix is ill-conditioned.   
 The solution has not converged.  Please check for rigid body motions   
 in your model.                                                         
                                                                        

 *** ERROR ***                           CP =     710.625   TIME= 183:29
 Preconditioned conjugate gradient solver error level 1.  Please check  
 for an insufficiently constrained model.  Switching to the sparse      
 direct solver may allow this nonlinear analysis to continue beyond     
 this point.                                                            
    >>> NEGATIVE PIVOT ENCOUNTERED
 *** LOAD STEP    30   SUBSTEP     1  NOT COMPLETED.  CUM ITER =    188
 *** BEGIN BISECTION NUMBER   8    NEW TIME INCREMENT=   3.1396   

     FORCE CONVERGENCE VALUE  =   3554.      CRITERION=  0.5102E-04
    >>> Thermal expansion factor =  1.000000E-08

 *** WARNING ***                         CP =     728.203   TIME= 183:46
 The PCG solver detects that the stiffness matrix is ill-conditioned.   
 The solution has not converged.  Please check for rigid body motions   
 in your model.                                                         
                                                                        

 *** ERROR ***                           CP =     728.203   TIME= 183:46
 Preconditioned conjugate gradient solver error level 1.  Please check  
 for an insufficiently constrained model.  Switching to the sparse      
 direct solver may allow this nonlinear analysis to continue beyond     
 this point.                                                            
    >>> NEGATIVE PIVOT ENCOUNTERED
 *** LOAD STEP    30   SUBSTEP     1  NOT COMPLETED.  CUM ITER =    189
 *** BEGIN BISECTION NUMBER   9    NEW TIME INCREMENT=   1.5698   

     FORCE CONVERGENCE VALUE  =   3554.      CRITERION=  0.5102E-04
    >>> Thermal expansion factor =  1.000000E-09

 *** WARNING ***                         CP =     746.047   TIME= 184:04
 The PCG solver detects that the stiffness matrix is ill-conditioned.   
 The solution has not converged.  Please check for rigid body motions   
 in your model.                                                         
                                                                        

 *** ERROR ***                           CP =     746.047   TIME= 184:04
 Preconditioned conjugate gradient solver error level 1.  Please check  
 for an insufficiently constrained model.  Switching to the sparse      
 direct solver may allow this nonlinear analysis to continue beyond     
 this point.                                                            
    >>> NEGATIVE PIVOT ENCOUNTERED
 *** LOAD STEP    30   SUBSTEP     1  NOT COMPLETED.  CUM ITER =    190
 *** BEGIN BISECTION NUMBER  10    NEW TIME INCREMENT=   1.0000   

     FORCE CONVERGENCE VALUE  =   3554.      CRITERION=  0.5102E-04
    >>> Thermal expansion factor =  1.000000E-10

 *** WARNING ***                         CP =     766.672   TIME= 184:25
 The PCG solver detects that the stiffness matrix is ill-conditioned.   
 The solution has not converged.  Please check for rigid body motions   
 in your model.                                                         
                                                                        

 *** ERROR ***                           CP =     766.672   TIME= 184:25
 Preconditioned conjugate gradient solver error level 1.  Please check  
 for an insufficiently constrained model.  Switching to the sparse      
 direct solver may allow this nonlinear analysis to continue beyond     
 this point.                                                            
    >>> NEGATIVE PIVOT ENCOUNTERED
 *** LOAD STEP    30   SUBSTEP     1  NOT COMPLETED.  CUM ITER =    191
 *** BEGIN BISECTION NUMBER  11    NEW TIME INCREMENT=   1.0000   

 *** WARNING ***                         CP =     766.734   TIME= 184:25
 The unconverged solution (identified as time 2497.78711 substep 999999)
 is output for analysis debug purposes.  Results should not be used for 
 any other purpose.                                                     




         R E S T A R T   I N F O R M A T I O N

 REASON FOR TERMINATION. . . . . . . . . .ERROR IN ELEMENT FORMULATION           
 FILES NEEDED FOR RESTARTING . . . . . . .  file0.R
                                            file.ldhi
                                            file.rdb
 TIME OF LAST SOLUTION . . . . . . . . . .  1694.1   
    TIME AT START OF THE LOAD STEP . . . .  1694.1   
    TIME AT END OF THE LOAD STEP . . . . .  2497.8   

 ALL CURRENT ANSYS DATA WRITTEN TO FILE NAME= file.db
  FOR POSSIBLE RESUME FROM THIS POINT




 *** NOTE ***                            CP =     766.891   TIME= 184:26
 During this loadstep the PCG iterative solver took more than 1000      
 iterations to solve the system of equations.  In the future it may be  
 more efficient to choose a direct solver, such as the SPARSE solver,   
 for this analysis.                                                     


 NUMBER OF WARNING MESSAGES ENCOUNTERED=         17
 NUMBER OF ERROR   MESSAGES ENCOUNTERED=         11



 ***** PROBLEM TERMINATED BY INDICATED ERROR(S) OR BY END OF INPUT DATA *****

+

---

D I S T R I B U T E D   A N S Y S   S T A T I S T I C S

---

+

Release: Release 19.1       Build: 19.1       Update: UP20180418   Platform: WINDOWS x64
Date Run: 08/11/2018   Time: 184     Process ID: 22568
Operating System: Windows 10  (Build: 17134)

Processor Model: Intel(R) Core(TM) i7-6700HQ CPU @ 2.60GHz

Compiler: Intel(R) FORTRAN Compiler Version 17.0.4  (Build: 20170411)
          Intel(R) C/C++ Compiler Version 17.0.4  (Build: 20170411)
          Intel(R) Math Kernel Library Version 2017.0.3 Product Build 20170413

Number of machines requested            :    1
Total number of cores available         :    8
Number of physical cores available      :    4
Number of processes requested           :    4
Number of threads per process requested :    1
Total number of cores requested         :    4 (Distributed Memory Parallel)              
MPI Type: INTELMPI
MPI Version: Intel(R) MPI Library 2017 Update 3 for Windows* OS


GPU Acceleration: Not Requested

Job Name: file0
Input File: dummy.dat

  Core                Machine Name   Working Directory
 

---

     0             DESKTOP-KUOGR22   E:Aerospace and Mechanical Engineering softwaresAdditive Simulation fileslearningfine mesh_ProjectScratchScrCAB4
     1             DESKTOP-KUOGR22   E:Aerospace and Mechanical Engineering softwaresAdditive Simulation fileslearningfine mesh_ProjectScratchScrCAB4
     2             DESKTOP-KUOGR22   E:Aerospace and Mechanical Engineering softwaresAdditive Simulation fileslearningfine mesh_ProjectScratchScrCAB4
     3             DESKTOP-KUOGR22   E:Aerospace and Mechanical Engineering softwaresAdditive Simulation fileslearningfine mesh_ProjectScratchScrCAB4
 
Latency time from master to core     1 =    2.639 microseconds
Latency time from master to core     2 =    2.082 microseconds
Latency time from master to core     3 =    2.566 microseconds
 
Communication speed from master to core     1 =  4314.83 MB/sec
Communication speed from master to core     2 =  2722.49 MB/sec
Communication speed from master to core     3 =  3334.30 MB/sec

Total CPU time for main thread                    :      769.6 seconds
Total CPU time summed for all threads             :      770.6 seconds

Elapsed time spent pre-processing model (/PREP7)  :        0.1 seconds
Elapsed time spent solution - preprocessing       :        0.6 seconds
Elapsed time spent computing solution             :      782.9 seconds
Elapsed time spent solution - postprocessing      :        5.9 seconds
Elapsed time spent post-processing model (/POST1) :        0.0 seconds
 
Equation solver used                              :            PCG (symmetric)
Equation solver computational rate                :       10.4 Gflops

Maximum total memory used                         :      258.0 MB
Maximum total memory allocated                    :     5184.0 MB
Total physical memory available                   :         16 GB

+

---

E N D   D I S T R I B U T E D   A N S Y S   S T A T I S T I C S

---

+


 *

---

*
 |                                                                           |
 |                       DISTRIBUTED ANSYS RUN COMPLETED                     |
 |                                                                           |
 |

---

|
 |                                                                           |
 | Ansys Release 19.1          Build 19.1         UP20180418     WINDOWS x64 |
 |                                                                           |
 |

---

|
 |                                                                           |
 | Database Requested(-db)  1024 MB    Scratch Memory Requested      1024 MB |
 | Maximum Database Used      22 MB    Maximum Scratch Memory Used     67 MB |
 |                                                                           |
 |

---

|
 |                                                                           |
 |        CP Time      (sec) =        770.594       Time  =  1842        |
 |        Elapsed Time (sec) =        793.000       Date  =  08/11/2018      |
 |                                                                           |
 *

---

*

 

Best,

Ashish

[Sandeep Medikonda]

Ashish,

  Can you include the following command snippets and set up a run?

amstep,build,,,4        !This will use 4 Time steps when heating is applied
amstep,build,,,,4       !This will use 4 Time Steps between layer additions
amstep,cooldown,,,40    !This will use 40 substeps for the cooldown process

 

If this doesn't work, check the 'ds.dat' file in the solver files directory and report back what additive commands are being used?

Look for keywords that start with 'am***' such as ambuild, amstep etc.

Regards,

Sandeep

[Sandeep Medikonda]

Also, try a case by constraining the face where the 3 selected nodes are on the side face, So like on the smaller cross-section face in your first post?

[ashish35]

Sandeep,

I got the problem resolved as I removed the contact region generated between the interface of part and support. Thank you for your help.

However, now I am trying to get the distorted part with built in stresses (without the baseplate and support) and applying external load on it to get the superimposed stress values. Could you please suggest me how can I proceed for this task?

Best,

Ashish

[Sandeep Medikonda]

Did you have to kill the contact? I am curious as you would need contact between them during the AM steps right?

[ashish35]

Sandeep,

Yes, it seems contact region between base and build is sufficient to successfully complete the AM removal step.

Actually I tried taking my part and assigning the support structure automatically from ANSYS (not defining the support through a CAD model), and I noticed that the automated wizard that ANSYS AM has does not create contact region between part and support (but it does between part and base interface).

So, with this observation, I deleted the contact region between the support configuration that I had and the part. It surprisingly didn't give me any rigid body motions. I really have no clue how.

Best,

Ashish

[Sandeep Medikonda]

Ashish,

  Try to use the direct solver when you see convergence problems in the base removal step.

   Introducing additional contacts is unnecessary when using the Wizard which overrides an internally created build-support contact.

  Just FYI: A colleague of mine has pointed out that all manually created (i.e. not the internally created build-support) contacts are killed on base removal step. This bug is rectified in R19.2.

P.S: If you have found a solution to your initial query, please mark it as a solution (even if it is your own post) so that it would make things easier for someone going through it at a later time.

Regards,

Sandeep

[ashish35]

Sandeep,

My instincts were telling me that it was a bug. Thank you for your help.

Best,

Ashish