Thickness reduction Shells.

[ajordanc]

I`m using ANSYS 6.1 Universitary version, up to now we don`t have available ls-dyna, so I have been trying to obtain some results of the following problem using ANSYS.

-12 step Sheet Metal forming, taking in account, material, geometric, contact non linearities and transient analysis.
-I have used shell 51 (axisimetric) and shell 181.

As far as I know shell 181 supports Thickness reductions, but I dont know how can I check this information during postprocessing.

Due to the fact that metal forming operation is held in 12 steps I wonder if ANSYS can use the deformed shape information to start with a new analysis, obviously taking in account the stresses and strains of the previous analysis.

Thank you in advance

 

[Drej]

Ajordanc,

I think you're correct in assuming that shell thickness reduction is supported for 181, as it is stated here:

http://www1.ansys.com/customer/content/documentation/60/Hlp_E_SHELL181.html

To check this in post-pro, you will need to create an etable input, see:

http://www1.ansys.com/customer/content/documentation/60/Hlp_C_ETABLE.html

and specify SMISC,17 in it. If you start a new analysis, ANSYS will ignore any previous results (hence, "New Analysis&quot, but it is possible to read or "restart" from a previous load step, which will give you your desired result. To do this, enter:

/solu

then

solve

using your first load step, then resume the db you just used to solve with:


resu,<dbname>,db

Remember: If used in SOLUTION, this command is valid only within the first load step.

then create your &quot;new&quot; load step (using &quot;lswrite,#&quot; if necessary) and issue:

ANTYPE,,REST

and then issue &quot;solv&quot; (or &quot;lssolve,# if necessary) as normal.

See:

http://www1.ansys.com/customer/content/documentation/60/Hlp_G_BAS3_12.html

Hope this helps
-- drej --

 

[ajordanc]

Drej:

Thank you for the info is exactly what I needed, I already gotten some results of the thickness reductions using shell 181, now I want to compare shell results with solid 185 results but I´m not getting convergence with it.

I haven´t tried with the second topic (restart the analysis) because I don´t have the tool geometries by now, but I´m sure that is going to work, you are good at it!

We have now available LS-DYNA, maybe somebody can tell me
which one is the difference between explicit and implicit time integration?, that as far as I know explicit corresponds to LS-DYNA and implicit to ANSYS.

Thanks for your time

 

[juzz]

Hello, ajordanc!

About the differences between implicit and explicit time integration you could find an idea in LS-Dyna Guide appendix A. subsection 1. (&quot;Comparison of Implicit and Explicit Methods&quot; - &quot;Time Integration&quot or in Theoretical Manual Chapter &quot;Time integration&quot;
If you need to find more information the best choice is a very good book: &quot;Nonlinear Finite Element Analysis&quot; (or something like that - I don't have the book at my office right now) by Ted Belytschko (which is one of the gurus of Dyna).
Anyway, you'll see that LS-Dyna is more suitable to your needs than Ansys.

I hope these will help you

Best regards,
Juzz
-----------------------------
Justin Onisoru
Researcher
Romanian Academy,
Institute of Solid Mechanics
-----------------------------

 

[ajordanc]

Hi Drej, I got the tool drawings, I have been trying with the instructions you gave me, but I couldn´t get good results, I have a doubt, you wrote:

then create your &quot;new&quot; load step (using &quot;lswrite,#&quot; if necessary) and issue:...

In this part, I have to erase the first die and punch and create the second pair of tools, to get the second deformed shape, am I correct? then, I have to start with the second pair of tools and the deformed shape of the first pair.

Please answer.

Best regards,

Ad

 

[Drej]

STEPS:

1. Setup geometry of model, Boundary Conditions etc as per normal including your first load step
2. Solve (solv)
3. Finish (fini)
4. Enter solution (/solu)
5. Resume from the database you created in step (2)
6. Indicate to ANSYS you would like to do a restart analysis (ANTYPE,,REST)
7. Enter the appropriate environment (/prep7 /solu etc) and specify revised (i.e. your next load step) or additional loads as needed. Remember to ensure that any previous loads are removed if you don't want them!
8. Specify whether your old .tri file is to be used (kuse)
9. Enter solution and solve

For additional load steps, repeat steps 7 to 9 or use the load step file method to create and solve multiple load steps. Use the following commands:

lswrite
lssolve

Try it just with two load steps at first (try an easy load case) then continue with the harder stuff.

A sample restart input listing for you:

! Restart run:
/FILNAME,... ! Jobname
RESUME
/SOLU
ANTYPE,,REST ! Specify restart of previous analysis
!
! Specify new loads, new load step options, etc.
! Take appropriate corrective action for nonlinear analyses.
!
SOLVE ! Initiate restart solution
SAVE ! Optional SAVE for possible subsequent singleframe restart
FINISH
!
! Postprocess as desired
!
/EXIT,NOSAV

See:

http://www1.ansys.com/customer/content/documentation/60/Hlp_C_ANTYPE.html

Good luck!
-- drej --

 

[ajordanc]

Hello All, I have been trying to do the second load step but almost at the beginning of it, the analysis stops due to this error

*** ERROR *** CP= 14342.844 TIME= 13:09:08
DOF (e.g. Displacement) limit exceeded at time 1.1
(load step 2 substep 1 equilibrium iteration 6)
Max.absolute value= 2291798.69 (limit= 1000000) at ROTZ of node 927 .

In the first load step I applied a displacement of 1.5 inch, the second one was zero displacement.

Does anyone have a hint ?