Exporting stress results from Print3D to Optistruct

ks prasanna

Hello, I am working on Fatigue analysis of 3d printed parts.

I want to export residual stresses from Print3D simulation as preloads into Optistruct. 

How to map the results? 

Thanks!

 

Here is the screenshot of the FE model. 

Fig: Print3D Displacement contour

Amith Anoop Kumar

Basically do you want to export this results to optistruct. I think the best way would be tocheck which all file formts can be imported in optistrct and convert your presnt file into that format. 

Is there any other way I am not sure though

ks prasanna

The result h3d file has only von-Mises stress contour. 

How to get tensor values ? 

please help ASAP

Amith Anoop Kumar

ks prasanna said:

The result h3d file has only von-Mises stress contour. 

How to get tensor values ? 

please help ASAP

Basicaly whatever you request in output block you will get too see in h3d file

Angel Limon

ks prasanna said:

The result h3d file has only von-Mises stress contour. 

How to get tensor values ? 

please help ASAP

Hello,

The Inspire Print analysis run does not request the full stress tensor. You could modify the Radioss engine file keywords from the Inspire Print run manually and then re-run via the compute console. These files are in your run folder and can be opened from your run history. From there you can map the print stresses to a new mesh for use in Optistruct as an initial condition.

Solver files in run history: https://2021.help.altair.com/2021.1/inspire/en_us/topics/shared/analysis/run_history_t_2.htm

 

Radioss Engine Keywords: https://2021.help.altair.com/2021/hwsolvers/rad/topics/solvers/rad/animation_post_process_h3d_output_r.htm

Mapping Process using SimLab:

1.) Import the Radioss solver input file into SimLab , choose “create a solution”.
2.) Then attach the h3d results to the solution (Note the Radioss solution created upon import is not run ready from SimLab , it’s just a place to hold the results for the mapping tool.)

3.) Import your Optistruct mesh into SimLab and create a nonlinear static solution using that mesh.
4.) Use the mapping tool to map the results from the appropriate Radioss body to your Optistruct mesh body, select “Create a Load” and this will generate an initial condition in your Optistruct Solution.

 

 

I hope that helps,

Angel

ks prasanna

Angel Limon said:

Hello,

The Inspire Print analysis run does not request the full stress tensor. You could modify the Radioss engine file keywords from the Inspire Print run manually and then re-run via the compute console. These files are in your run folder and can be opened from your run history. From there you can map the print stresses to a new mesh for use in Optistruct as an initial condition.

Solver files in run history: https://2021.help.altair.com/2021.1/inspire/en_us/topics/shared/analysis/run_history_t_2.htm

 

Radioss Engine Keywords: https://2021.help.altair.com/2021/hwsolvers/rad/topics/solvers/rad/animation_post_process_h3d_output_r.htm

Mapping Process using SimLab:

1.) Import the Radioss solver input file into SimLab , choose “create a solution”.
2.) Then attach the h3d results to the solution (Note the Radioss solution created upon import is not run ready from SimLab , it’s just a place to hold the results for the mapping tool.)

3.) Import your Optistruct mesh into SimLab and create a nonlinear static solution using that mesh.
4.) Use the mapping tool to map the results from the appropriate Radioss body to your Optistruct mesh body, select “Create a Load” and this will generate an initial condition in your Optistruct Solution.

 

 

I hope that helps,

Angel

Hello Angel Limon,

 

Thanks for the reply. I will try following the steps. 

ks prasanna

Angel Limon said:

Hello,

The Inspire Print analysis run does not request the full stress tensor. You could modify the Radioss engine file keywords from the Inspire Print run manually and then re-run via the compute console. These files are in your run folder and can be opened from your run history. From there you can map the print stresses to a new mesh for use in Optistruct as an initial condition.

Solver files in run history: https://2021.help.altair.com/2021.1/inspire/en_us/topics/shared/analysis/run_history_t_2.htm

 

Radioss Engine Keywords: https://2021.help.altair.com/2021/hwsolvers/rad/topics/solvers/rad/animation_post_process_h3d_output_r.htm

Mapping Process using SimLab:

1.) Import the Radioss solver input file into SimLab , choose “create a solution”.
2.) Then attach the h3d results to the solution (Note the Radioss solution created upon import is not run ready from SimLab , it’s just a place to hold the results for the mapping tool.)

3.) Import your Optistruct mesh into SimLab and create a nonlinear static solution using that mesh.
4.) Use the mapping tool to map the results from the appropriate Radioss body to your Optistruct mesh body, select “Create a Load” and this will generate an initial condition in your Optistruct Solution.

 

 

I hope that helps,

Angel

As per the discussion with Angel, I added the line

"/H3D/NODA/GPS"  to Rad files and rerun on Compute.

I am able to get the GP stress tensor values

droccaforte

Hi KS,

There are multiple engine files for each phase of the print simulation.  The last one is the one you will need to add the desired stress keywords.  I think that is why you did not see them.  If you want to use element rather than nodal stress that is all covered here:

https://2021.help.altair.com/2021/hwsolvers/rad/topics/solvers/rad/animation_post_process_h3d_output_r.htm

With regards to generating an h3d for import into hyperlife:  Rather than using the ascii import into HV and generating an H3D from HyperView I would just use the mapped stresses as an initial condition on a nonlinear stress run. Constrain the outer faces and solve.  You will then get an h3d results with the stress tensor you can import to Hyperlife.

 

Cheers,

 

-Dave