Contact problem during rigid pole impact analysis

HYOJUNG KIM

Hi. I'm doing a analysis using RADIOSS solver.

I analysis about rigid pole impact and the model composed to 4 components and one rigid pole.  

The cover and side components are connected  by bolting and I use rigid and spring elements to describe bolt connect.

And the tie constraint(Contact Type 2) are used to model to connect base and side componets.

But the analysis stop due to contact error.

How can I solve this problem?

 

Please help me  and I attach my RAD file. 

Thank you.

 

 

 

HM50_0000.rad

PaulAltair

You have several issues I can see,

1: you have one tied interface (bottom plate to beam) where there are shared nodes with rigid bodies, that isn't allowed with 'standard' formulation, you need to switch to Spotflag 27

2: your 2nd tied interface has only main side defined (and it is bottom plate again) with no secondary nodes (changed to top plate and added the secondary nodes)

3: You have your main nodes of your RBODY connected to mesh (should be free)

4: Your bolts have a density 1000x too high (reduced to steel)

5: Your spring bolts have 0 stiffness in all directions (set them to 1k translational, 100 rotational)

6: Your spring bolts have 0 mass or inertia set, I set arbitrary values for them

7: I think like the last model you sent, you had set almost no parameters at all in the Type7 contact (for gapmin etc) I set recommended values

8: Your geometry seems odd?, Your lower plate is coincident with the beam, there should really be self contact in the panel, but you can't define it if you have it set up like this

 

I attached my version, it goes through starter now, but I didn't run the engine so you may have more work to do! The only warnings in starter are for tied interface nodes remaining with bad projections.

(You didn't share your engine 0001.rad so I made one up, can you share them in future please? It is easier to debug your model if I can see how you are running it!)

Hope this helps,

Paul

PS_001.zip