Altair RISE

A program to recognize and reward our most engaged community members

Nominate Yourself Now!

I am stuck and need help

I am completely new to Hyperworks. I have been reading all kind of ebooks to understand and i have to simulate a 3 point bending as a start. Then i ll do optimizations on hyperstudy. Size and Shape optimizations.

To do that first i need a successful radioss run. Which i get a lot of errors. A LOT. I dont have any idea how to get a successful run.

In Summary I have followed these steps.

1. Create the Components

2. material (Non Linear Materials MAT2 or MAT36)

3. Properties (PShell)

4. Load Collector (Imposed Velocity of Impactor / Fixed Boundary counditions etc)

5. Contact (Interface Type 7 between Supports and Inner / Impactor and Outer and Self contacts)

6. Output Block

7. Engine Cards.

in attachments you can find the model. I would be really appriciated if someone helps me with that.

Unable to find an attachment - read this blog

Find more posts tagged with

English

Radioss

Accepted answers

All comments

Simon Križnik

Hi @leozzy

There are a couple tutorials about 3pt bending: RD-T: 3060 Three Point Bending & RD-T: 3595 Three Point Bending with HyperMesh. Optistruct would be better suited for size & shape optimization IMHO, but it could also be done with Hyperstudy for learning purposes. Note that optimization can also be done in Radioss, see RD-E: 5100 Optimization in RADIOSS.

To debug models use Tools>Model Checker>Radioss Block and check runname_000.out file

The following corrections were done on your model:

-components were assigned Part card image

-shell elements were created with QUAD4N element types, which are only used for 2D analysis. To update element types compatible with 3D analysis: 2D>elem types>2D&3D and make sure quad4 is set to shell4N then select all elements and update

-load collector 'Impactor Velocity' did not have node group assigned- assign the same group used for 'Impactor Constraints' and was acting in the wrong direction (Z instead of Y)

-rigid elements were badly defined. To create 1D>rigids>create>set multiple nodes 2-n and calculate primary node

-ouput block data_var parameter was undefined. click the table and enter: DEF for default ouput request

These are my recommendations:

-contact definition was modified

-additional output blocks were defined for rigid impactor and midspan node, which can be useful to plot force vs. displacement in HyperGrapg (see attached image)

-the pillars are probably attached to reinforcements so I defined a type 2 tied interface, but there are many more options to connect components (1D>connectors)

-the model could be simplified with planar quarter symmetry that would improve computational efficiency, which is important if you want to perform multiple runs.

-Advanced Mass Scaling (AMS & AMS/DT control cards) could be used to speed up beyond DT/NODA/CST, but for some reason there is large negative energy

<?xml version="1.0" encoding="UTF-8"?>

Unable to find an attachment - read this blog

leozzy

Sorry for late reply. I thank you too much for your kind help. i didnt have time to sit down and check your corrections. Now i am checking and i understand your points. I ll use different type of connectors after optimizations to see its effect on stress, strain and most importantly on mass.

Are you familiar with Hyperstudy as well? I need to use hyperstudy to simulate all crosssections in one simulation by using hypervolume variables.

Simon Križnik

I am familiar with basic functionalities in HyperStudy, but not enough practical experience to give useful advice. But you can open a topic in HS forum.

There is a free ebook and also some HS videos on Altair Germany.

leozzy

Could You pls give me a hint how did you plot this chart? X type y type what should i choose?

<?xml version="1.0" encoding="UTF-8"?>I am stuck

Simon Križnik

Usually, the displacement is plotted on the X-axis and force on Y-axis. So just switch components accordingly. Then apply -1 scale factor on X component, because Y displacements are in the negative direction in global coordinate system. If you have planar symmetry (half or quarter) you should also scale Y component by 2 and 4 respectively to compensate for the model reduction.

The same can also be achieved with cross-plot functionality in HG.

<?xml version="1.0" encoding="UTF-8"?>

Unable to find an attachment - read this blog

leozzy

Thanks for the help once again. I have learnt how cross plots work. Thanks i ll use them later on when i am gonna do comparisons. I have one more question.

In the Resultant displacement it show 75 m (for midspannode outer pillar) and 35 m (midspannode inner pillar) respectively. Between outer pillar and inner pillar is just 60 mm. How is that even possible?

<?xml version="1.0" encoding="UTF-8"?>

Simon Križnik

That's a good question.

There is localized buckling (more deformation) of outer pillar component in contact with the impactor due to compressive stress and the inner pillar does not buckle, because it is loaded only by tensile stress. In this image blue is compressive and red is tensile stress.

<?xml version="1.0" encoding="UTF-8"?>

There is also a weak coupling between the pillars unlike for example I-beam or solid beam which deform more uniformly.

To post-process strains define control card ENG/ANIM/SHELL/TENS/STRAIN and set Istrain=1 on properties of interest. In HW plot strain>signedvonmises.

Unable to find an attachment - read this blog