Jump to content
Jan Grasmannsdorf

Definition of Revolute Joints in OptiStruct

Recommended Posts

Dear Mr. Grasmannsdorf,

I would like to ask how to define Revolute Joints for an FE Analysis with OptiStruct. I modelled a Shaft which should be constrained in a mounting, except for the revolution around the shaft axis. What would be the appropriate way to model this constraint?

I used two Rigid Spiders within the shaft and mounting and a revolute joint to connect the rigids. However in simulation the model seems to be unconstrained and is not kept at its location. What do I need to consider when modelling revolute joints or how else could I model the desired constraint?


Mit freundlichen Grüßen


Share this post

Link to post
Share on other sites



in your model, you used the Joint of Type "JOINT", which is meant for Multibody (Kinematic) analysis only. Therefore, currently your shaft and mounting are not connected via the joint.

To consider a revolute joint in FEM (Static), you should use the joint type "JOINTG", which is defined in the same way and menu in HyperMesh, except for the option "FE" instead of "MBD". To Model the JOINTG within your model, you also need to define a local coordinate system prior to modelling the joint.

Here is a flash video, how to do so:

Unable to display content. Adobe Flash is required.


Share this post

Link to post
Share on other sites

In addition, there are some more issues in your model:

1) the "bellkrank nondesign" parts are not connected to the shaft (2D mesh hits a 3D mesh, but there is no connection made) . Therefore no load is transmitted via this interface. I recommend to use a TIE Contact between the two parts.

2) The "rotation" of the shaft in the mounting will not transfer any load from the shaft to the SPC at the end of the mounting. You will get a rigid body mode. I would suggest to use a Slide Contact between the Shaft and the mounting, instead of the "Rigid + Revolute Joint".

Another approach would be to use "Multibody dynamics" in solidThinking Inspire and model the kinematic behaviour first. After this, the resulting forces could be mapped to the single parts and then used for optimization.

Share this post

Link to post
Share on other sites

Join the conversation

You can post now and register later. If you have an account, sign in now to post with your account.

You are posting as a guest. If you have an account, please sign in.
Reply to this topic...

×   Pasted as rich text.   Paste as plain text instead

  Only 75 emoji are allowed.

×   Your link has been automatically embedded.   Display as a link instead

×   Your previous content has been restored.   Clear editor

×   You cannot paste images directly. Upload or insert images from URL.

  • Create New...