Jump to content
Sign in to follow this  
Dirk76

Visualize shell thickness in Hyperview

Recommended Posts

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.

Share this post


Link to post
Share on other sites

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.

Share this post


Link to post
Share on other sites
On 10.10.2017 at 8:57 AM, Q.Nguyen-Dai 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?

Share this post


Link to post
Share on other sites

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 .

Share this post


Link to post
Share on other sites
On 4/19/2018 at 3:17 PM, alex_ander 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.

Share this post


Link to post
Share on other sites

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:

hv_shell_thickness.png.9d4914a1d40bc8add0578e63e1fcb9e6.png

 

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

 

Share this post


Link to post
Share on other sites

Create an account or sign in to comment

You need to be a member in order to leave a comment

Create an account

Sign up for a new account in our community. It's easy!

Register a new account

Sign in

Already have an account? Sign in here.

Sign In Now
Sign in to follow this  

×