Can Nastran create a constraint in a single direction (fixed in the positive x direction, free in the negative x direction)

[roy7BB24]

Hi All, 

Just a question regarding setting up constraints in Nastran. The bottom surface of an assembly is free to slide and separate from the face of the component it rests on, and I would like to show this behavior in the analysis. Obviously, a separation w/ sliding contact would work, but makes the run times a lot more significant - is there a way to place a constraint so that the nodes on the surface are free to displace in the +y direction, but aren't able to displace in the -y direction? 

Kind Regards

Roydon Mackay

[John_Holtz]

Hi Roydon.

The answer is no: there is no constraint type that prevents motion in one direction (positive) but allows motion in the opposite direction (negative).

If such a constraint existed, it would still solve using an iterative technique to determine which nodes are "in contact" and which have separated. The runtime would not be that much faster than using a part with separation contact. (Of course, modeling the extra part takes some time depending on the complexity.) If the constrained face is a flat plane, the "floor" could be shell elements with the largest mesh size possible. One element is sufficient. (If you make it solid, you need a minimum of 6 elements, assuming the mesher does not require more elements.)

John

[roy7BB24]

Hi John, Thanks for that, 

I just had a few questions as per the best way to set this up?

Please see attached a rudimentary sketch of what I'm modelling. All components here have been idealized as surfaces.

1. Is there an optimum distance to model the floor plane from the base of the beam? I assume they can't be on the same plane, 1mm lower should do the trick right? And as part of this I would just set my penetration surface offset to be this same value.

2. In terms of the exact way to set up the constraint -

 a) symmetric or unsymetric?

b) which item should be the primary entity?

c) Specifying the max activation distance? I expect deflection somewhere in the vicinity of 50mm at this stage of the analysis, in addition if I follow your advice and specify an exceptionally high mesh size for this part I might wind up with a activation distance of 3m or there abouts?

3. In terms of mesh control, I've found when I try to create a mesh control that's coarser than the global setting, it meshes as per the finer control, in this case the global control. At this stage the model is a single part consisting of multiple surfaces and one or two bodies, so I can't use the mesh table to control a specific part. If there an easy way to do this or is the only option to set a mesh control on every other surface except for the floor surface?

EDIT: I think I've solved 3, I'm going to model the floor sheet as a separate part, and create an assembly so I can control the floor sheet using the mesh table

Kind Regards

Roydon Mackay

[John_Holtz · Accepted solution]

Hi Roydon,

1. is correct. Use a small gap for convenience and set the Penetration Surface Offset to the same value. Note that it may be necessary to have the normal direction for the floor and the normal direction for the bottom flange facing each other. In the Model Tree, right-click "Elements > Normal Display > Vector" or "Color". The arrows need to face each other, or yellow needs to face yellow.

2. I would make the floor the primary and penetration type Unsymmetric Contact. (This limits the contact elements to be from the nodes on the secondary, the flange, to the elements on the primary, the floor.) The maximum activation distance needs to be 1.1 to 1.2 times larger than the mesh size on the primary.

The constraints on the beam need to resist the load and provide static stability. 

3. The "Mesh Control" should be named "Mesh Refinement" because it can only refine the mesh. Therefore, you put the refinement on the beam and use the global mesh setting to set the size for the floor.

John

[roy7BB24]

Thanks for the assist, the analysis is starting to behave as expected.

1. Any idea where I'd find more resources on what normal direction for shell idealizations does/impacts. I haven't come across this before and would like a better understanding of what I'm tweaking and when I should be changing this going forward.

2. I noticed when I run the analysis like this I get about 10 000 G3051 warnings - it says on the warning that no action is normally required. I also noticed that when I change the penetration offset from 6mm(exact) to 5.99 it drops to about 2000. I assume that its caused by slight numerical errors when the nodes are created "inside' the separation constraint, and the program is adjusting the mesh to solve this? Any recommended action or this isn't something you'd normally worry about

3. Lastly I've noticed some slightly strange behavior is the model. I've tried a different method, creating all my thin bodies as surfaces in inventor, and the creating shell idealization's and assigning thickness's. As the whole thing is one welded assembly (except for the single separation contact), I've just created a solver contact - offset bonded, unsymmetric, activation distance - 20mm (just ran a global mesh size of 15mm for the part, might be slightly large, will refine as the analysis improves). 

I've attached a snip of what looks like the behavior that causing trouble - I've modelled PFC as three surfaces, as the top and bottom flanges are a different thickness to the web, however the solver contact doesn't appear to detect that these three surfaces are intended to be 'welded'. Is this an error in how I've set this up, or is the solver contact never intended to pick up this type of join? 

[John_Holtz]

For 1, the last third of this article on knowledge.autodesk.com discusses what can happen if the contact is through the wrong side. See Understanding maximum activation distance and contact type in a Simulation. (Some of that discussion is related to thin solid parts and some is related to shells.) 

For 2, the G3051 warnings indicate the nodes on the secondary are penetrating the faces on the primary. The position of the node is moved to eliminate the interference. If the interference is insignificant, then the node is moved an insignificant amount and it is not a problem. If the interference is large, then the mesh will be distorted by moving the nodes. See Tip 44 in the PDF document attached to my forum post Suggested Reading - Tips and Tricks on the Inventor Nastran forum.

For 3, an activation distance of 20 mm for solver contact is huge. See Tips 16, 18 and 19. In short, the activation distance with solver contact is slightly larger than the gap between the items being bonded (offset bonded in the case of shell elements).

Since you created the surfaces manually, is it true that there are no gaps between the edge (of the web for example) and the matching surface (of the flange for example)? If there are no gaps, you should try to mesh the model using "Continuous Meshing". If Continuous Meshing is successful, then no contact will be needed. (Continuous meshing matches the nodes between different faces so that the load is transferred from element to element through the node. Contact replaces continuous meshing so that the load is transferred from element to element through the contact that connects the adjacent nodes and faces.) 

I just looked up PFC. If that stands for Parallel Flange Channel, Inventor 2024 will create the three faces of the channel by extruding the 3 lines that define the mid-surface. The three faces create one surface body which Nastran meshes as a continuous part. There is no need for continuous meshing or contact. (Of course, continuous meshing or contact may be necessary for connecting different members of the structure.) I don't know if older versions of Inventor also create a single surface body for an extruded channel or if they create multiple surface bodies. Multiple surface bodies are what requires continuous meshing or contact.

John

[roy7BB24]

1. I've had a look at that article. I noticed at the very end there was a note that if a manual contact is applied to an element, the solver will not create a connection to that element. After some further testing it seems like the solver will not create any contacts to the secondary contact but will pick up the primary (hopefully I don't have that the wrong way round), so that explains why I was having the problem with that lower flange unbinding. 

 See the figure from the page that was linked, I just wanted to confirm, if the normal direction on part 3 was reversed, there would be no way to create a connection between part 2 and part 3, with either a solver or a manual contact. 

Lastly, I had a lot of crashes when I tried to view or change the normal planes, I noticed it was worse when I tried to show the planes as colors as opposed to the vectors, anything that will help with that?

I know in the past when I've tried to create a mid-surface from a PFC section that was created in frame generator, inventor creates the mid-surface, however as its one shell idealization, all three faces have the same thickness, which often isn't an assumption that can be made, I think for example 200 PFC will have a flange thickness of 12mm and a web thickness of 6mm. This is one of the primary reasons I've been experimenting with creating the surface manually and creating separate idealizations for the web and the flange.