keep rigid connectivity between parts

[Mofy]

Hi.
I've a problem of keeping the structure intact during the impact simulation of two different parts. I used connector elements "weld" to weld these parts together but t the moment of impact the parts look as not having any rigid connection between them. Any help is appreciated.

 

[akabarten]

Hi,

If your parts are connected but do not have equvivalence mesh then you can use tie connection (*TIE).
If you have a gap between the parts you can setup rigid body with specific nodes from both parts (*RIGID BODY, TIE NSET).

Regards,
Bartosz

 

[Mofy]

Thank you Bartosz for your reply.
Could you please explain, in more details how can do the 2nd choice when I have a gap between two parts that constitute an assembly?

Regards,

Mofy

 

[akabarten]

Hi,

Create a node set to define regions you want to connect.
The node set needs to include nodes from both parts.
Next use the node set to setup a rigid body.
In an inputdeck it will be looks like:

**
** node set for rigid body
*NSET, NSET=rigid_connection-NSET
 ...
 list of nodes
 ...
**
** define rigid body
*RIGID BODY, REF NODE=1, TIE NSET=rigid_connection-NSET, POSITION=CENTER OF MASS
**

Regards,
Bartosz

 

[Mofy]

Thank you Bartosz for your reply.

The main problem in this task is when I tried to connect two tubes to another third tube at two different locations. In fact I did not write the code but I'm using the interaction module to draw and analysis the model.
Here what I did: I defined reference points on the three tubes, then I used constraints feature to constrain one reference point on each of the first two tube and two RPs on the third tube. After that I used a connector (weld)to connect the each RP point on the 1st two tubes to their corresponding RP on the third tube. Is this the right way to connect the tubes. From your reply my method seemed not OK (I'm a new user of Abaqus). Your comment please.

Regards,

Mofy

 

[akabarten]

Hi,

This is how I would do it:

1. Go to "Interaction" module
2. Tools -> Reference Point
Position should be somewhere in the middle of region you want to connect,
but it is not very important since Abaqus will move due to point 6.
2. Constraint -> Create -> Rigid Body -> Continue
3. Choose Tie (nodes) as type of rigid body
4. Choose regions to connect, nodes or geometry (depend what do you have).
You can make multiple selection with Shift.
5. Assign the reference point from step 2
6. Mark "Adjust point to center of mass at start of analysis"

Repeat the process for each connection location.

Regards,
Bartosz

 

[Mofy]

Hi.

I followed the steps that you mentioned but the following error preventing the running of the model. errorNode 40 instance front cross-1 belongs to more than one rigid body). This means that we can only connect two different parts at the same time. In my case I cannot connect two tubes to the same third tube even at different locations.


Regards,

Mofy

 

[akabarten]

Hi,

Does any of your parts is rigid?
I was thinking all three parts are deformable.

Regards,
Bartosz

 

[Mofy]

Hi,

All three parts are deformable.

Regards,

Mofy

 

[akabarten]

Hi,

That was fast ... 5 minuts

Maybe I am missing something. You have three parts and want to connect them in two diffrent regions.
As long the regions does not overlap each other you should get no error.

Maybe you can make some sketch, print screen, or share the model?

Regards,
Bartosz

 

[Mofy]

Hi Bartosz,

Please see the attachment below for the tubes that are not overlapped. It is a SIMPLE assembly.

Regards,

Mofy

 

[akabarten]

Hi,

I made a sketch, did you try in this way?

Bartosz

 

[Mofy]

Hi. Bartosz,

Thank you for your help.

As I told you that I am a new user. My interpretation to your sketch is: I have to draw the sketches (circles) on new datum plane, then constrain (tie) it to the outer surfaces of both tubes, But what is about the reference point that I should define?
If I used rigid body constraint then the complier will show an error that the horizontal tube cannot be constrained to more than one rigid body. Am I right?

Thank you for your time.

Mofy

 

[akabarten]

Hi,

Please take a look for attached model.
I connected three tubes like on your sketch with two rigid bodies, I have no error.

Regards,
Bartosz

 

[Mofy]

Hi.

I appreciate your help. If you do not mind can you convert the file from version 6.12 to ver 6.11. This because I was not able to open it in my version. When I converted it it thing was shown in the screen.

Regards,

Mofy

 

[Mofy]

Hi Bartosz,

Thank you for you help. There is no need to convert the file to ver. 6.11 because I imported the input file. It works perfectly.

May you help by answering the following question: if I've a point that represent the center of gravity of a part (which has a mass) and a part from the tube but I want to connect it to the tube using connector (e.g. beam). How can I do that?

Regards,

Mofy