Hypermesh error warning 1284 and 1931

Rahul_P1

Hi,
many thanks for your reply.
yes I think I do the good work.
My erros are the followings:

*** WARNING # 1284
No SPC or SUPORT1 data specified for static SUBCASE 1.
Make sure the model is constrained otherwise.

*** WARNING # 1284
No SPC or SUPORT1 data specified for static SUBCASE 2.
Make sure the model is constrained otherwise.
*** WARNING 1931: SPC 1 is not referenced by Case Control.
*** WARNING 1931: LOAD 1 is not referenced by Case Control.

I have :
- 3 load collectors (in SPC load collector, I put Load and I tick the the forces; and for the two forces I tick none) isn't it ?
- 2 load steps (subcase 1 and 2, I just create without add anything partucarly)

The problem maybe comes from I put my boundaries conditions on node/point which do reference to several nodes.
like in the picture

And maybe I don't parameter very well this option. Could you indicate me the procedure to follow ?

Many thanks per advance,

Best regards,

BM

PS: when you post a quick response could we add picture ? and not have to create a new discussion ?

Rahul_P1

BM,

Given your two kind of forces and constraints I believe this should be your procedure,

Create three load collectors, all three should have no card image.
In one load collector put your x forces, in the other the y forces and in the third load collector put your boundary conditions i.e. constraints.
In your first subcase select the load collector with the x forces in the LOAD section and the load collector with the boundary conditions in the SPC section.
In your second subcase select the load collector with the y forces in the LOAD section and the load collector with the boundary conditions in the SPC section.

Linking your nodes with rigid elements and then constraining it is fine in principle, what link elements do you use in this hole?

To reply with images you can click on the reply button (blue button at the right hand bottom corner) this will open a reply window where you can reply with the images

Rahul_P1

Hi,
Thanks,
For the links between the center node and the others:
- I create two lines
- I create a node in the intersection
- I create connectors/spots and I specify in 'location': the center node and in 'what' I tick all the nodes of the diameter.

It seems I input correctly the three load collectors with none card.
But I still have the same mistake:

ANALYSIS RESULTS :
------------------

ITERATION 0

*** WARNING # 1955
Static Loadcase 1 has zero static force vector.
This typically produces zero solution and zero compliance.

(Scratch disk space usage for starting iteration = 44 MB)
(Running in-core solution)

Volume = 2.24286E+06 Mass = 3.36429E+00

Subcase Compliance
1 0.000000E+00

I input the loadstep as follows in the picture below:

Many thanks

BM

Rahul_P1

Benoit,

Do you need to constrain all the nodes in the circumference of your hole or just the four nodes?

Connectors is not the right option for this, you need to use rigids panel to create RBE 2 elements connecting nodes from the circumference of the circle with the node at the centre. Then constrain the centre node as you wish.

Rahul_P1

yes, I need to constrain all the element around the hole.
What is the procedure ?
1 create a node at the center
2 create a connector on this node
3 link the connector with the elements ?

Rahul_P1

Benoit,

To constrain all the nodes around the circumference of the circle, go to rigids panel, change the independent node to calculate node (click on the downward arrow and change to calculate node) and the dependent node selector to multiple nodes.

then select all the nodes around the circumference of the circle, HyperMesh will automatically create a node at the centre and create rbe 2 elements as required. you can then create a constraint on the centre node and all the circumferential nodes will be constrained as well.

Your error also indicates that perhaps the force is not properly defined, the force must act on a node, the error suggests that the force is not applied on an fe entity, please recreate the force on a node.

Rahul_P1

Before your last message, I try to apply my constraints anf force directly on the model and it works correctly !!
So you 're right, my forces and my constraints sere not well established on node.
So I am following your way but where is the rigid panel ? I am on V11 ?
Many thanks,
Benoit

Rahul_P1

Good it works !!many thanks !