Elemental Non Linear strain output vector

[milani]

Dear all,

I would recovery elemental strain on shell element in Autodesk Nastran. How can I obtain it?

With  output vector 712 shell max von mises top /bottom, I can recovery nodal strain. 

Is possibile to create an elemental strain output vector?

Regards

Stefano

[Andrew.Sartorelli]

Hi @milani,

You should have also receive the shell elemental max von mises strain top/bottom under vector 6108. You can find a list of all of the elemental result vectors for shell elements in our online help.

Regards,

Andrew

[milani]

In output results I don't obtain this vector. Actually I uses 2015 version. Is a problem? How can I request this vector?

Thanks 

S

[Andrew.Sartorelli]

Hi @milani,

OK, that does give some hints. In 2015 (and NEi versions) we could only output stress or strain in the same analysis. Do you have both STRESS and STRAIN in your case control like shown below?

SUBCASE 1
   SPC  = 1
   LOAD = 1
   STRAIN(PLOT,CORNER) = ALL
   STRESS(PLOT,CORNER) = ALL

 If so, try with just STRAIN:

SUBCASE 1
   SPC  = 1
   LOAD = 1
   STRAIN(PLOT,CORNER) = ALL

Here is a quick link to the help on the STRAIN case control command.

Andrew

______________________________________________________________

If my post answers your question, please click the "Accept as Solution" button. This helps everyone find answers more quickly!

[milani]

I have this initial condition. Strain are required.

Stefano

[Andrew.Sartorelli · Accepted solution]

Hi @milani,

You will need to remove STRESS from your case control section. We only support requesting both STRESS and STRAIN in Autodesk Nastran 2016 and newer.

Regards,

Andrew

______________________________________________________________

If my post answers your question, please click the "Accept as Solution" button. This helps everyone find answers more quickly!

[milani]

i'll install nastran 2017

Thanks

Stefano

[Andrew.Sartorelli · Accepted solution]

Hi @milani,

Be sure that you also install the 2017 R1 pack from the product enhancement section on the Account portal also. We added a new contact algorithm that is enabled through the ENHCCONTACTRSLT parameter that really helps for hertzian contact!

Enjoy the rest of your weekend!

Cheers,

Andrew

[milani]

Really interesting! Thanks for your Sunday support!

Good Work

Stefano

[milani]

I re-open this discussion because I have a related problem. I need to obtain the only the non linear component  for shell element.

This ouput can be obtained by 7088 and 7488 vector?

How can I obtain  the residual stress and strain for shell element after load removing? 

Best regards

Stefano

[Andrew.Sartorelli · Accepted solution]

Hi @milani,

That is correct, 7088 and 7488 will show only the non-linear component. But for a quick double-check, run a small test where some elements enter the plastic region. You should see all of the elements not in the plastic region with a value of 0 for these vectors, while the elements with plastic strain will have a non-zero value.

Once you remove the load, the typical stress and strain vectors should then have none-zero values if elements have entered into plasticity.

Cheers,

Andrew