## Recommended Posts

Hi，I have a question，

In Optistruct, how to apply a displacement load on a cylindrical rigid wall to simulate a three-point bending test like following picture？

##### Share on other sites

You can refer attached OptiStruct example. For enforced displacement you can use SPCD card.

3-Point Bending using RBODY.pdf

3Point_Bending_RBODY.fem

Simon Križnik likes this

##### Share on other sites

Thanks，@Rahul R

I use SPCD card for a simple example,but it doesn't work, I am puzzled why？

plate_tension_SPCD.fem

##### Share on other sites

In loadstep subcase section , you checked IC condition as SPCD. Its not needed for static run. Just deactivate and run again.

##### Share on other sites

Thanks，@Rahul R

I am so sorry I don't express it clearly，I want to apply a uniform displacement=80mm to the rigid cylinder in the Y—axis direction winthin 0.2s，like this

but I don't know how to make it by Optistruct？

##### Share on other sites

the B-pillar three-point bend problem would require non-linear quasistatic or dynamic analysis due to three major nonlinearities:

-large displacements/rotations/deformations

-material yielding

-contacts

In dynamic analysis, inertial effects and momentum are included (loading in 0.2s) while quasistatic simulates very slow movement.

Please go through free eBook: Introduction to Nonlinear Finite Element Analysis using OptiStruct

The following videos should help:

Try to replicate in your model the analysis setup from the example shared by @Rahul R

##### Share on other sites

Thank you@Ivan,

There is still a problem here in the example shared by In Optistruct, how to set a cylinder created by myself as a rigid body and apply speed, I want to extract the contact force generated during the collision, and the rigid wall inside Optistruct cannot extract the contact force.

Or in an explicit nonlinear dynamics analysis, can RW in load steps use other geometry as a rigid wall?

I did a simple example，but there is no contact force in .h3d file，can you check it？thanks in advance

following is.fem file

##### Share on other sites

In your shared deck, you have loadstep set to linear static analysis. CONTF will not work for linear cases.

##### Share on other sites

In Optistruct, how to set a cylinder created by myself as a rigid body and apply speed, I want to extract the contact force generated during the col﻿lision, and the rigid wall inside Optistruct cannot ﻿extract the conta﻿ct force.

2

Create rigid body using 1D>rigids. Boundary conditions are applied on the master/independent node. Output requests like displacements, forces,... can be requested by Analysis>output block.

##### Share on other sites

There is still a small problem here, which makes me very confused. I originally applied a forced displacement of 80mm in the direction of the dof2 y axis, but the analysis result is that the rigid body has a large displacement along the x-axis direction. I don’t understand what went wrong. here is .fem file , can you give me some suggestion?

And how to extract the value of specific energy absorption instead of cloud image?

##### Share on other sites

Create a rigid body on impactor cylinder and then constrain its independent/master node in all DOF and apply the SPCD on the same node.

Attached is the edited model. Check the modifications and compare to 3pt bend example. The analysis takes a lot of iterations to converge so perhaps there is a more efficient analysis setup.

ESE in the global output request will output strain energy and strain energy density.

steel_20kN_SPCD_edit1.hm

steel_20kN_SPCD_edit1.h3d

## Join the conversation

You can post now and register later. If you have an account, sign in now to post with your account.

×   Pasted as rich text.   Paste as plain text instead

Only 75 emoji are allowed.