Hi, I'm using the sol 200 for a st

[nastrmsc]

Hi,
I'm using the sol 200 for a structural optimization but I have problem with the stress responses.
I've used four type of DRESP1:
1) DRESP1 198 S198 STRESS PSHELL 9 198
2)DRESP1 1198 S198 STRESS PSHELL 17 198
3)DRESP1 6 S6 STRESS PBARL 7 6
4)DRESP1 6 S6 STRESS PBARL 7 6

for more than two property.
Linked to these responses I have DCONSTR like this:
DCONSTR 4000 198 233.

where 233 MPa is the upper bound for von mises stress.
I found inconsistencies between the stress responses that appear at the end of the file f06(the list of active responses) and the stresses related to the last analysis, the one with the optimized configuration .

In fact if I check one element in the stress responses list(figure3) and after in the static analysis(figure 4), I find a different value of stress. Can you tall me why?

I don't hunderstand why the optimization finishes with hard convergence (figure 1)but I've still elements that violate the constraints.
Thanks.
Best regards

 

[dmapguru]

The stress output in figure 3 shows the Component No. column with a value of 17 for both elements 20008573 and 20008574. In figure 4, the grey line you have highlighted is for the Z1 shell surface, not Z2. If you look at the Z2 line (second line for each shell), this corresponds to Z2. For element 20008573 we see a MAJOR stress of 1.396058E+02 which is consistent with the VALUE column in the STRESS RESPONSE output of figure 3, which is showing 1.3961E+02 (rounded up). The same is true for element 2008574. What does your case control command for STRESS output look like. Did you request the CORNER or BILIN option?

Also you said you still have elements that violate the constraint. This violation is not included in the output you show. Post your .f06 file if you want me to look in more detail.

DG

 

[nastrmsc]

Hi,
unfortunatly I can't show you the f06.
If I understood correctly my response for the CQUAD4 is not for the von mises stress but for the principal stress(even if I've used the correct stress item code).
My model is made up of PSHELL(CTRIA3 and CQUAD4) andPBARL(CBAR) elements.
and for those elements I don't have any problem: the stress in the 'active stress responses' list(at the end of the final report of f06) is the same of the static analysis.
How can I constraint the von mises stress for CQUAD element? because it seams I've used the wrong card.
This is the stress request:
STRESS(SORT1,REAL,VONMISES)=ALL

I've done some analysis changing into:
STRESS(SORT1,REAL,CENTER,VONMISES)=ALL
STRESS(SORT1,REAL,CORNER,VONMISES)=ALL
OR STRESS(SORT1,REAL,BILIN,VONMISES)=ALL

but I had the same problems.
Thank you a lot.
Best regards

 

[dmapguru]

Without the detailed information of the .f06, I can only guess.

Do you see *** USER WARNING MESSAGE 6418 (SDR2A) anywhere in the f06 file?

Something is aligning item code 17 to the MAJOR principal stress, which is the correct item code for this item when CORNER stresses are active. For example, do you have another output request that asks for CORNER output (like FORCE or STRAIN) - this will give UWM 6418.

When CORNER stress (and force, strain) are requested, you must look at the item codes for CQUAD4(144) - here, item code 17 is Z2 major principal; I suspect you are looking at the item codes for CQUAD4(33) where item code 17 is the Z2 von Mises stress.

Why can't you show the .f06 file? Is the model confidential? If yes, build a small basic model that has the same essential attributes as your confidential model (and will therefore exhibit the same curious behaviour), and post that model.

DG

 

[nastrmsc]

Yes there was the error you wrote.
And the problem was exactly that one you told me.
In my Command section there was another output for the FORCE sets to BILIN.
Now evrything is ok and the stress item code on the response (DRESP1) is that one I want.
Thank you very much for your help!!!
Best regards