Visualize shell thickness in Hyperview

Altair Forum User

Hi all,

 

for a certain purpose I do have to make a cross-section of a plate made up with shell elements. Now I know how to do it but I was thinking, is there a way to visualize the actual shell thickness in Hyperview? It is possible to do it?

 

Thanks in advance.

Altair Forum User

Hi,

It is not possible to visualize the shell thickness in HyperView, as of now. But this feature will be updated in the coming versions.

Q.Nguyen-Dai

I make a script to write down (SAMCEF's) shell thickness into HWASCII format for visualizing within Hyperview. It works well /emoticons/default_smile.png' srcset='/emoticons/smile@2x.png 2x' title=':)' width='20' /> 

Altair Forum User

Thanks guys for the response.

 

I need it because I wanted to see delamination, since the classical contact gap in HV doesn't work for me and I really don't know why... maybe my solver is too old.

 

I think I have to do it in LS Prepost.

Altair Forum User

Visualize shell thickness in Hyperview is possible in HyperWorks 2017 version?

Altair Forum User

Hi,

This option is not available yet in HyperView.

Q.Nguyen-Dai

A small TCL script to export thickness information into HWASCII format from Hypermesh and you can visualize within Hyperview no problem.

 

Altair Forum User

can i get it ?how to use it ?

alex_ander

Altair Forum User said:

A small TCL script to export thickness information into HWASCII format from Hypermesh and you can visualize within Hyperview no problem.

 

 

Hi Q.Nguyen-Dai.

 

Could I please get it from you?

Altair Forum User

Hi,

is it  possible to visualize the shell thickness in HyperView in Hyperview 2017. As you replied earlier that in the coming versions it would be updated .

Q.Nguyen-Dai

Altair Forum User said:

 

Hi Q.Nguyen-Dai.

 

Could I please get it from you?

 

Yes, it's possible. Share me your Hypermesh model with some shell elems. I'll test it before to show you.

Q.Nguyen-Dai

If you have HM model with shell elements, thickness is defined via component property, you can test the following code:

 *createmarkpanel comps 1 'Select Component' set mycomps [hm_getmark comps 1] hm_markclear comps 1;  set myHMDir [file dirname [hm_info hmfilename]] set outFile 'thickness.hwascii' set fileTypes { {'HWASCII' {.hwascii} }     {'All files' *} }  set fileName  [ tk_getSaveFile -filetypes $fileTypes \ -title 'HWASCII data' \     -initialdir $myHMDir \     -initialfile $outFile ]  set fh [ open $fileName w ]  puts $fh 'ALTAIR ASCII FILE' puts $fh '\$TITLE = Static Analysis' puts $fh '\$SUBCASE = 1 Subcase 1' puts $fh '\$BINDING = ELEMENT' puts $fh '\$COLUMN_INFO = ENTITY_ID' puts $fh '\$RESULT_TYPE = Thickness(s)' puts $fh '\$DELIMITER = ;'  foreach i $mycomps { set cname [hm_entityinfo name components $i] set elems [hm_elemlist id $cname] set prop [ hm_getvalue comps id=$i dataname=propertyid ] set thickness [ hm_getentityvalue props $prop \$PSHELL_T 0 ]; #puts [format '%d %s %d T=%0.3f' $i $cname $prop $thickness] foreach eid $elems { puts $fh [format '%d;%0.6E' $eid $thickness] } }  close $fh;

If this macro was executed successfully, you get a file 'thickness.hwascii'. Export your FE model to Optistruct format for example, you got 'mesh.fem'.

Within Hyperview, load 'mesh.fem' & 'thickness.hwascii', you can visualize the shell thickness now.

Here's my screenshot:

 

Note: My script was tested with NASTRAN profile. Maybe you need some adaptation for another profile.