Altair RISE

A program to recognize and reward our most engaged community members

Nominate Yourself Now!

contact master slave in optistruct

priyankabhola

Hi,

i am doing analysisin optistruct

project detail as per following.

load body (load caring vehicles).

payload 37ton apx.

traget: i want to test strength for floor members . not only floor even all side walls of vehicles. can sastain the load.

problem: master --dummy weight in 3d mesh 37 ton. 2.) slave: load body mesh part. but master weight run out of load body .connect not work properly betwen body and dummny weight.weight goes out of side walls .please help. i dont want to apply pressure or force because at a time it work either on floor or side wall of load body. i want dummy weight will work at a time all sides (floor side and front and rear wall)

file attached for ref.

With regards

priyanka

Unable to find an attachment - read this blog

Find more posts tagged with

English

OptiStruct

Accepted answers

All comments

FaroukM

Hi,

i am doing analysisin optistruct

project detail as per following.

load body (load caring vehicles).

payload 37ton apx.

traget: i want to test strength for floor members . not only floor even all side walls of vehicles. can sastain the load.

problem: master --dummy weight in 3d mesh 37 ton. 2.) slave: load body mesh part. but master weight run out of load body .connect not work properly betwen body and dummny weight.weight goes out of side walls .please help. i dont want to apply pressure or force because at a time it work either on floor or side wall of load body. i want dummy weight will work at a time all sides (floor side and front and rear wall)

file attached for ref.

With regards

priyanka

Hi,

I opened your model. Your master ELSET is empty (there is 0 element) :

image.png.f16a68755634784645213eb1dafcb176.png

I have a question for you : Why are you using Linear Static step ? Why not Non Linear Quasi-Static ?

Best regards,

Unable to find an attachment - read this blog

priyankabhola

Hello,

Thanks for your reply,

actually reason for using linear static is time save i just want to check the total stress on floor for optimization first .

if it will behave ok and after that i want to go for non linear.

can you guide me or help for non linear for the same project.

boundary condition or deck setup.

or share some tutorial.

with regards

priyanka

priyankabhola

Hello,

Today i run same file with modification as per error suggested by you in snapshot ..missing master element but still my vehicle not run properly.

regards

priyanka

Unable to find an attachment - read this blog

Simon Križnik

Hi,

there are several issues in your model:

the payload is modeled with shell elements, but solid element would be more appropriate. The upper surface shell would sag under gravity and its weight would be transferred only by side shell surfaces. Solid elements would equally distribute the weight over the floor.
the 'lc6' load collector referenced in linear static load step is empty, which is invalid (the solver will error out). Reference a gravity load collector '0.1_z negi' instead.
the master component is usually stiffer or in case of equal stiffness the one with the coarser mesh. In your case, the cargo has the same stiffness and mesh size as a steel cargo box, but I would still choose the cargo as a slave.
Sliding contact might not work using linear static analysis. In linear static analysis, the contact status does not change, does not slide and the contact stiffness is constant. Freeze Contact enforces zero relative motion on the contact surface, the contact gap opening remains fixed at the original value and the sliding distance is forced to be zero. Additionally, rotations at the slave node are matched to the rotations of the master patch. The FREEZE condition applies to all respective contact elements, regardless of whether they are open or closed. Freeze Contact can be activated using TYPE=FREEZE on the CONTACT, MU1=FREEZE on the PCONT entry or by using the Penalty-based Tied Contact. Penalty-based tied contact is activated by using the TIE entry for the contact interface (with CONTPRM,TIE,PENALTY, the default).