Cancel
Showing results for 
Search instead for 
Did you mean: 

Fatal Message - No Surfaces or edges Defined for Contact/Glue Region

Experimenter
Experimenter

I have a model where I am taking a slice of a bolted system and doing an analysis with symmetry. It has been giving me a few headaches, unfortunately I can’t share the model so I made a simple test case to check things.

 

When trying to put some elements into a group to use to apply a load I select a surface but it says there are no elements available to select. Yet I can do the same thing and select nodes on the surface.  (an example in this model is Surface 3 at the end of the bolt. I added the nodes to Group 4, but I can’t add any elements via Element/On Surface).  I know of many other ways that I can add the elements, but I want to know why it won’t let me do it this way.

 

I have a similar issue with the contact. I go and specify contact areas by surface, but when I run the model I get “User Fatal Message 4690 (SCTFCRL)   No Surfaces or edges Defined for Contact/Glue Region”.  I can go and specify the contact via nodes or, hopefully, by element faces, but if I update the mesh I have to redefine the contact.  I have gone in and tried to associate the elements with the surface but it says that there are no eligible elements to associate, they are either the wrong type or already attached.

Can anyone help clarify why I am having these issues using surfaces? My reasearch has not been turning up anything useful.

 

Thank you,

 

Rob

3 REPLIES

Re: Fatal Message - No Surfaces or edges Defined for Contact/Glue Region

Siemens Genius Siemens Genius
Siemens Genius

How did you mesh this geometry? It looks like the elements are not associated with geometry. 

 

After looking at your model, it appears you have coincident nodes along curve 34 down to the bottom of the bolt. So I started out by using the command Tools > Check > Coincident Nodes, select all and okay. 
Curve with coinc nodes.JPG

Then use the command Modify > Associativity > Automatic, select one on the element in the bolt and use the "Pick" and "Add All Connected Elements". 
Pick all connected.jpg
Click OK and select the bolt geometry and click OK again. When prompted for a search tolerance divide the default by 2. 

 

Use Modify > Associativity > Automatic again for the block with the bolt hole. Select one element in the block and use Pick and Add All Connected. Select the geometry of the block and use the default tolerance.  

The analysis should now run.

Re: Fatal Message - No Surfaces or edges Defined for Contact/Glue Region

Experimenter
Experimenter

Giampietro,

 

Thank you for the reply. 

 

I meshed the 'base' via Size on Solid, then adjusted the Size on Curve for a few places. For the bolt I cut it and specified the mesh along the lines of the symmetry face, mesh surfacem then revolved it deleting the original mesh. I filled in the center in the same way, with an extrude along node path, then added the 2 solids back together  (sorry, I neglected to merge coincident nodes in this quick model).

 

I had previously tried to specify the associativity of the elements / faces on the surface (via Modify > Associativity > Elements) to the solid but had no luck, while this seems to work fine whendoing the 'Automatic' option. Was it likely just a poor flow on my part that prevented proper association? Is there a way I can mesh, or build the model, so I don't have to go back through and associate the meshes on the individual components?

Everything on that simple model worked just fine, so I will give it a shot on my other model and report back.

 

Rob

Re: Fatal Message - No Surfaces or edges Defined for Contact/Glue Region

Experimenter
Experimenter

Giampietro,

 

Everythign on my full model ran just fine, but I have a bit of a follow on question about associativity - I had some issues with nodes that were being used for preload. There is a rigid element connecting the nodes of the nut that are on the symmetry plane (~half of the highlighted nodes in the image) to the center. These rigid elements have symmetry defined in a CS along the bolt axis, which is not aligned with any global CS, but is along the face of the bolt. The same was done for the bolt. Again, this was following something that was done by someone else previously.

 

The remainder of the nodes on the face of the nut are connected to the same central node, but in 1-6, not symmetry. Again, the same applies for the nodes along that interface on the bolt. Trying to run the model would give an error that the highlighted nodes were improperly constrained, which makes sense since they effectively have 2 sets of constraints on them, even though the constraints are constraining the same things, just in different form.

I removed the highlighted nodes from associativity with all bodies and the model runs fine. Is that the proper way to do it, or might that have other unintended consequences? I know I could remove the rigid elements from those edge nodes, but I am trying to get a better understanding of associativity.