Glued connection - normal modes - long solve time - is glued (weld) contact the problem?

Pioneer
Pioneer

Hi - I think this is my first post here, but I've often found useful tips, thank you!

 

My question:

I have a simple model comprising a concrete raft foundation modelled in tets and a couple of small cylindrical pedestals, also in tets, that I want to glue to the top of the raft. 95% of the elements are in the raft, about 70,000 in total. I've used Connect|Automatic menu with default settings and Glue Type = Weld, eval order = high, refine source = Refinement ocurs, penalty factor units = scale factor, scalefactor = 1.

 

This seems to work well enough. However, the solution time for the raft with the two pedestals glued-on is about three times longer (4 minutes) than for the raft by itself (ie no glue or pedestals).

 

When I extend my model to include more glued connections (about 20) and beams and plates (about 50% more nodes added in total), the run times blow out even more - normal modes takes more than an hour. A modal frequency response runs for more than 6 hours with no solution.

 

I suspect the glue is the problem - can anyone offer any tips to resolve this problem?

 

Many thanks

Steve

2 REPLIES 2
Highlighted

Re: Glued connection - normal modes - long solve time - is glued (weld) contact the problem?

Gears Phenom Gears Phenom
Gears Phenom
Generally a normal modes and FREQ response using a solid model with require extensive time compared to using soley sheels and beams, are the TETS 10 nodes or 4, there are some methods that can help:

First of all try and reduce the total number of DOF, if the geometry is simple mesh in HEX no mid size nodes.

Secondly check your search distance for Glued Connection and you can also reduce the actual region size.

Re: Glued connection - normal modes - long solve time - is glued (weld) contact the problem?

Siemens Phenom Siemens Phenom
Siemens Phenom

Solve time is basically related to the number of DOF's squared. So as you increase the number of nodes/dof's, solution time does not increase linearly but exponentially. The next factor you are seeing, solid elements only have 3 dofs/node, while beams and shells have 6 dof's/node, so adding stick and shell nodes, makes the dof count increase even faster than adding solid element nodes.

The next factor is the density of the stiffness matrix, in other words "how interconnected" the model is; adding glue connections or things like rigid elements and mpc equations can have a significant effect on the density and therefore take more resources, memory and time.

 

If your solution is taking too long, the f04 file has all of the information needed to understand where the time is going(what modules), what resources are being used and if you may benefit from changing resource settings in Nastran.

 

Regards,

Joe