Learning Forum

[Kaushal Sawant]

I have a door and a hinge assembly, to which I have applied a joint load. The hinge is bolted to a pillar which is defined by Body-ground connection, while the door is connected to the hinge in bod-body fixed connection type. The hinge and the bush is connected via revolute joint to ascertain the revolution. 

Boundary conditions:

1. Body-body joints:
1. Fixed joints given between ‘Hinge and pillar’ and ‘hinge bush and door’.
2. Revolute type of joint given between hinge bush and hinge.
3. Hinge pin is suppressed.
2. Body – ground joint:
1. The pillar is grounded using ‘Body-ground’ joint.
2. Mesh size: 2mm, refined at hinge and bush.
3. Material assigned: Structural steel for all.
   

Detailed description:

1. The similar analysis is carried using rigid body dynamics, however, we cannot get stress information, hence we used staic structural analysis.
2. Static analysis was carried initially using the large deflection ‘off’. However, there was unrealistically large deformation. Also the stress values were large.
3. Hence, I turned on large deflection. However, it creates error, “distorted element”. I checked the element using “Mesh by ID” option. For every analysis, the distorted element. was in the hinge bush. 
4. If I tend to refine the mesh, I get not enough memory error.
   
   

Action taken for above errors:

1. Applied load with large number of sub steps i.e. keep auto time stepping turned on with 20,10 and 500 as initial, min and max sub steps.
2. Turned on iterative solver for convergence errors.
3. Simplified the hinge bush model by removing the holes.

In spite of taking above actions, the error persists. 

Error which shows distortion in part



If the mesh is refined, then less memory error.


Description of parts


Any help is highly appreciated, as the above analysis is timeline critical

[Kaushal Sawant]

Description of joints

[peteroznewman]

 

To solve the running out of memory error, open the Geometry in SpaceClaim and on the Prepare tab, use the Midsurface button to replace the Door solid body with a midsurface.  Create two planes above and below the Hinge Leaf and on the Design tab, use Split Body on the Pillar and remove most of the length of the pillar. In Mechanical, apply Fixed Supports to the two new cut faces. This will greatly reduce the number of elements and allow you to use more elements on the hinge itself.

I would replace the revolute joint, unsuppress the pin and add Frictional Contact between the hinge bush, pin and hinge.

 

[Kaushal Sawant]

@peteroznewman, thank you so much for your reply. I have an update on the assembly. I have made the door and bush the 'rigid body' and made the hinge and pillar flexible. I was now able to get the stress value on the hinge leaf. The reason behind making the door rigid is that the door is made of structural steel having superior YTS and UTS, while hinge is made up of aluminium alloy, which is much less stiffer than the door. Also, hinge being the weak link and prone to much stress, this should be the area of interest. Took the reference from here:
https://forum.ansys.com/forums/topic/regarding-force-and-moment-in-ansys-static-structural/

I hope my understanding is correct.  Moreover I'll try doing the steps yopu mentioned above rerun the simulation

[Kaushal Sawant]

@peteroznewman, one question. How should I revolve the door around the hinge's axis if I remove revolute joint ? I have applied the remote displacement to door surface, and assigned the pillar (to which hinge, bush and door is connected) to fixed suppport. 

[peteroznewman]

Duplicate the analysis and use Part Transform to rotate the parts to different angles.

You could potentially create a Design Variable in SpaceClaim or DesignModeler to rotate the parts and have a single analysis with an Input and Output Parameter and a Table of Design Points to rotate the door to different angles.