Updating the Model - Sequence contains no matching Element

[martinjb]

Dear HyperSizer,

Hypersizer version - 6.4.52

I have run an analysis within Hypersizer and managed to get a range of thicknesses and cross sections for a number of panels. I would like to look at the displacements with PATRAN/NASTRAN. In order to do this I need to re-read the data back into Patran/Nastran via an updated .dat file (*_i01). In the older versions of Hypersizer the .PM1 was automatically created and stored within the location of the .dat & .f06 file. 

In 6.4.52 I have noticed that you only need to specify a 'FEM Filename(created by modeler) and FEA Force Result Output Filename(created by finite element analysis).  After reading the help file it points towards performing the FEM update via the Update button on the project setup form.  Having pressed the update FEM button i get an error message that says

Sequence contains no matching element
See log file for more detail
E:\.........\TEMP\HsFeInterface.ExportProperties.log

The attached file is a print out of the .log file

Sorry I cannot attach the .dat file as it sits on a separate network 

I have tried to methods of sending the model to Hypersizer.

• Exact copy of the Nastran output .bdf
• Breaking the .dat file into separate files (.GRID .LOAD .SHEL .TEMP etc.)

In both cases I still get the Sequence error message.  Do you have any ideas what I could have done wrong in setting up my Hypersizer run to cause the error?

I have analysed the Hypersizer tutorial files and an updated FEM file is created when it is asked for, hence why I feel the problem lies with my initial set up.
Thanks

[Ryan]

Does the project have any mechanical load sets? It is looking for a mechanical load set to get a default temperature for the component properties. It doesn't appear to the handle the case where all the load sets are thermal which may be causing the issue.

When you update the FEM 3 files are created: iteration FEM *_i.bdf (no more *_i##.bdf's in V6.4), *.PM1 and *.CEL1. The PM file contains the new materials and properties, the CEL contains the new element definitions, and the iteration FEM merges the PM and CEL files directly into a copy of the source FEM (include files are no longer used).

-Ryan

[martinjb]

Ryan,

After much searching and many different attempts, i believe that i have solved the problem.

I had initially created my .bdf and subsequent Subcases via Patran and then directly imported them into Hypersizer.  However having re-read the Hypersizer_PRO_O4.pdf I discovered a number of things that could be causing an issue. The main issue being, I was trying to output both mechanical and thermal loads in the same subcase.

SUBCASE 1
$ Subcase name : op1b_lc01
   SUBTITLE=op1b_lc01
   SPC = 81
   LOAD = 83
   TEMPERATURE(LOAD) = 60

I have now created two subcases within the .bdf

SUBCASE 1
$ Subcase name : op1b_lc01
   SUBTITLE=op1b_lc01_mech
   SPC = 81
   TEMPERATURE(LOAD) = 60
$
SUBCASE 2
$ Subcase name : op1b_lc01
   SUBTITLE=op1b_lc01_therm
   SPC = 81
   LOAD = 83

The two subcases have been imported into Hypersizer and then combined. The two LoadSets are combined into a single LoadCase that has subsequently analysed (along with other loadcases) and i have received updated  *_i.bdf, *.PM1 and *.CEL1 files.
 
Thank you for pointing me in the direction of my fault and i guess i should RTFM more. 

However, in the process of solving one problem, another question has arisen.  When adding temperature to the model does Hypersizer recognise the second line of the TEMPP1 Nastran card?
TEMPP1  10      1       200.
        2       THRU    10      15      THRU    22

Is there a way that i could check, that the elevated temperature is applied to my component and therefore subjected to a reduction in material properties? The only way i could find is to 'Analyze current component' and then look at the Temperature used in the Design-to-loads Tab.
 
To ensure that the TEMPP1 cards are applied to all the elements required i created a new card for each element -
TEMPP1  10      1       200.
TEMPP1  10      2       200.
TEMPP1  10      ..n     200.
TEMPP1  10      15      200.
TEMPP1  10      16      200.
TEMPP1  10      ..n     200.
 
Many thanks
Martin
 

[Ryan]

Thanks for the follow up. It looks like adding a mechanical load set is a workaround for the bug.

The THRU option is supported for the TEMPP1 entry. Make sure that there are continuation characters for the subsequent lines. You can also verify the element temperatures in the graphics using Data | FEA Loads | Element Temperature.

TEMPP1       201       1      1.                                        *
*        2       THRU    10      15      THRU    22     50

-Ryan