Chassis model seperating under explicit Dyanamic simulation, how to bond parts together 1

[RDelaCourt513]

Hello,

I want to analyse a the deformation of tubular space frame chassis on Abaqus under a crash scenario using explicit dynamics.

I have created the model on Solidworks using the weldment feature and imported the part into Abaqus as a parasolid file.

however upon completion of the run it appears that even though the chassis has been imported as one part the members are not connected together (it looks like the chassis has been inserted as an assembly.) I didn't think that I would have needed to worry about this.

Upon import of the part I selected the option to "combine into single part".

I have attached some snaps to show you what is happening, I am a fairly new user to Abaqus so I am still learning so any information would be greatly appreciated.

Thank you,

Ryan

 

[FEA way]

Just use tie constraints to connect all these parts together. You can even do it automatically, using Find contact pairs tool. Connections can be checked with eigenfrequency extraction analysis.

 

[RDelaCourt513]

Thanks for the advice, the chassis I have imported has been imported as once whole part as opposed to separate sections (which is why this is throwing me off) I have tried the tie constrain as you suggested but I have no luck, I have simplified the chassis structure for the moment and have only included the floor section and the rollcage.

I have attached an initial state and the 8th frame in, you can see that the cage section just separates from the attached section.

 

[FEA way]

Perform eigenfrequency extraction analysis before the actual impact study. If the first modes show that the bars are flying away it means that you need contraints.
Maybe automatic ties didn’t work here. Define them manually and make sure that the parts that don’t touch each other but are slightly separated will be connected (by changing tie adjustment tolerance).

You can also request unconnected_regions=yes during the job submission to generate sets with unconnected regions.

 

[RDelaCourt513]

Thank you for the advice. I will attempt to resolve this issue and get back to you.

 

[FEA way]

No problem. One more thing - make the mesh finer. Current one is too coarse and irregular.

Actually, I would model this using beam elements first.

 

[Mustaine3]

Let's say your geometries (tubes) are connected in Solidworks, but are standalone tubes after the transfer to A/CAE. Then you could try this:

Separate the tubes into separate parts
Part -> Copy -> Separate Disconnect Regions

Then you add all those new parts into a new assembly. This should now look like the whole structure again.
Now merge all the instances into one part.
Merge/Cut Instances

If this works, then you will have a new parts with all the tubes and they are geometrically connected to each other. That means, that after meshing you have common nodes between them and there is no need to tie tube together.

 

[RDelaCourt513]

Thanks for your input both, I am a new user to Abaqus so there is obviously a lot I am yet to learn.

FEA Way - Im assuming that there is a beam profile feature on Abaqus yes? The reason, my worry is that I would not be able to import my 3d sketch from Solidworks to use as a reference, I would have to create the sketch fresh ?

Mustaine3 - This seems like a good solution, I have in the past imported the model and it has come in separate parts. However i am now able to import the part so that it is one complete body (Stp file), in solidworks i created surfaces of the weldment members and imported the surface region into the step file supresses the solid bodies. this is why i am stumped, when i import the part into Abaqus I opt to "combine into single part". However it is still separating in the study.

 

[FEA way]

It should be possible to import wires(3D sketch) into Abaqus. In case of problems take a look at this post:

https://www.eng-tips.com/viewthread.cfm?qid=266450

 

[RDelaCourt513]

Thanks for this FEA way, this seems like a good soultion also as at least i know the geometry will be sufficient for use within the explicit solver (better that importing geometry from an external model at least.

I had a quick attempt at inmporting the sketch by means of a Step file but it did not work. I will have another try, Its good to know at least that it is possible.