Jump to content
exx077

Constraining a hole in limited DOFs

Recommended Posts

Hello,

 

I am looking to constrain a hole of a 3D model. I am currently using RBE2s (with all 6 DOFs on) within the hole and applying a constraint to the independent node in all 6 DOFs.

Doing this I am able to successfully run the optimisation.

 

However, I want to simulate a bar constraint where the model can rotate about the y axis but no others. I have tried deselecting the 5th DOF on both the RBE2s and constraint but this results in the optimisation failing.

How do I go about applying constraints to all DOFs but 5 (moment around the y-axis)?

 

Additionally, I am using RBE2s currently as I can apply a constraint to these. However, ideally I would be using RBE3s as these will better represent my problem. Is this possible to set up with the constraint in limited DOFs in mind?

 

Thank you

Share this post


Link to post
Share on other sites

Hello,

The difference between RBE2 and RBE3 is that RBE2 induces stiffness whereas RBE3 doesn't. If you need a stiff support, use RBE2; and use RBE3 for somewhat soft support.

It mainly depends on the type of analysis and your loading conditions you want to simulate.

Keep in mind RBE2 provides added stiffness.

There is a concept of independent and dependent nodes, which says that the motion from independent nodes will be transfered to the dependent nodes. If there is a single independent node, use RBE2. If there are a lot of independent nodes and one dependent node, use RBE3.

Thankyou

Share this post


Link to post
Share on other sites

I think your optimization running is failed due to rigid body motion, that is not enough constraint dofs

please share your fem file

Share this post


Link to post
Share on other sites

Thank you all for your responses.

 

@Toan Nguyen and @tinh, I will try and run the simulation for all DOFs selected on the RBE2s and all DOFs but 5 on the constraint.

 

 

@Sanjay Nainani your description of the differences between the use of RBE2 and RBE3's was very useful for me.

In regards to the following quote-

On 22/03/2018 at 5:41 AM, Sanjay Nainani said:

It mainly depends on the type of analysis and your loading conditions you want to simulate.

I would like to simulate a bolt that is contrained physically in space (DOFs 1,2,3) and contrained in rotation only in the x and z axis (DOFs 4,6), but can rotate about the y axis (DOF 5). I believe using RBE2s will induce an incorrect amount of stiffness to the hole. Is there a better way of approaching this problem?

 

 

Thank you in advance

Share this post


Link to post
Share on other sites

Hello @Sanjay Nainani,

 

I did not think it was possible to apply constraints to RBE3s as there is only one dependant node (and I thought you cannot apply a constraint to this).

Can you clarify?

 

Thank you

Share this post


Link to post
Share on other sites

Hello @Sanjay Nainani,

 

I have run into a few problems.

I set up the CBUSH element with 0 length. Using the 1st method explained by Tinh in the following thread.

https://forum.altairhyperworks.com/index.php?/topic/16708-creating-zero-length-cbush-elements-for-rbe3-support/

"it is very simply create CBUSH with non-zero length, then F3 > move node1 to node2 (check off "equivalence')"

 

I gave the CBUSH element the same PBUSH properties detailed in the link you provided.

5abe4d261376d_PBUSHProperties.PNG.283c6bb2f9fbf05598d4a1e080fc7319.PNG

 

 

The first problem I encountered was:

"*** ERROR # 339 ***
 The dependent d.o.f. is constrained by grid or spc data.
 RBE3 element id = 839109.
         grid id = 160922.
       component = 1.
 Number of bad RBE3 elements =        1"

Therefore, I made all the DOFs constrained to move past this till I had the simulation running.

 

The second problem was:

 "*** ERROR #  99 ***
  CBUSH element 839110 references incompatible PBUSH.
  K2/M2/B2, K3/M3/B3, K5/M5/B5, and K6/M6/B6 on PBUSH must be zero for
  CBUSH with no G0, CID, and blank X1, X2, and X3."

I have tried setting the value of K2, K3, K5 & K6 to 0 to resolve this. I have also tried setting all the values of K to rigid, but the same error (#99) occurs.

 

The problem that followed was:

"A fatal error has occurred during computations:
   *** ERROR #  40 ***
  CBUSH 839110 has zero length."

 

I am unsure on how to proceed from here.

 

Can anyone offer any advices to resolve these issues?

Thank you for your time in response.

 

Share this post


Link to post
Share on other sites

Hello all,

 

I did manage to resolve this. For all that come across this forum with the same issue, the following steps were used.

 

I received this error:

"*** ERROR # 5814 ***

The bushing element CBUSH 839110 has zero length. Please assign a coordinate

system to it using the CID field in its CBUSH card."

 

I changed the CID value to 0 in the input card, after following the instructions in the forum linked below:

https://forum.altairhyperworks.com/index.php?/topic/16708-creating-zero-length-cbush-elements-for-rbe3-support/

 

I changed all the K (1-6) values in the PBUSH property to RIGID.

 

This then allowed the simulation to run - although the convergence of the solution was questionable.

 

Thanks

Share this post


Link to post
Share on other sites

Create an account or sign in to comment

You need to be a member in order to leave a comment

Create an account

Sign up for a new account in our community. It's easy!

Register a new account

Sign in

Already have an account? Sign in here.

Sign In Now

×