Difficulty in establishing a connection between 2 surfaces (shell) in Prepomax


I’m facing a specific issue with my structural model of a ship, which I’ve simplified to main components such as the bulkhead and the hull in Rhino 3D. After exporting the model to PrePoMax using STEP or IGES formats, I’m struggling to establish effective tie connections between the bulkhead and hull surfaces.

Despite configuring tie contacts, the simulation results indicate that these connections are not functioning as intended. There’s a lack of force transfer and deformation, suggesting that the bulkhead and hull are not properly connected, which affects the structural integrity and the accuracy of the analysis.

Could anyone provide insights or recommendations on how to properly set up tie connections between the bulkhead and hull in PrePoMax? Are there specific settings or steps that I might be missing to ensure these components are fully integrated and interact correctly under load?

Thank you in advance for your help!

Did you try creating a compound part first ? If it doesn’t help, check the adjustment and tolerance settings of tie constraints. Then use a frequency analysis to easily verify the connections.

Yes, I have tried creating compound parts with several different ship models. Sometimes the compound is not created properly, or there are issues during the meshing phase, but these problems are quite rare. The usual issue is that the bulkheads are not meshed properly. I’ve tried increasing the tolerances to find all the connections, but then I encounter a ‘result fail’ error. Your suggestion to use frequency analysis to verify the connections seems logical, and I will try that as my next step. I am open to any further suggestions regarding tie settings and tolerances, as I would appreciate any additional advice you might have. I am feeling quite trapped in my current project and prefer using open-source solutions over other applications, as I support the expansion of these options.

Compound creation may sometimes fail due to small misalignments: Deformation in 2 or more bodies - #10 by Matej

You can also find some tips regarding tie constraints (tolerance, master/slave selection) here: *WARNING in gentiedmpc: no tied MP - #6 by FEAnalyst

The rules regarding master and slave selection are crucial. Most importantly, master should be the one with a coarser mesh.

“I’ve paid attention to the Master-Slave connections and manually entered the missing links. What should I do next?”

Try increasing the tolerance to make sure the surfaces that should be connected are within the range (measure the distance between the opposing nodes and add some additional distance just in case - nodes outside of the tolerance range are not connected at all) and using adjustment (this projects the slave nodes meeting the tolerance criterion to lie on the master surface).

It is not evident from the images if you are using shell geometry or solid geometry?

I am using shell elements. In fact, to make it easier to understand, I will leave the ship form and perform these analyses on a standard cylinder model. Then I will upload it here again with the simplified visual.

As you can see, I am also encountering errors with shell plates even in a simple geometry.

Can you share the file ?

If you’re using *TIE, beware that it doesn’t work reliably on shells:

It can only be used with 3-dimensional elements (no plane stress, plane strain, axisymmetric, beam or shell elements).

Use TIED contact instead.

Looking at the images, I would say the compound part is the way to go. I am wondering why it does not work. Can you share the .pmx file?

This quote from the documentation must be outdated because tie constraints can work normally with 2D elements. Maybe there could be some issues in particular cases but I haven’t encountered them yet.

You have too many parts for the deck:

The interference between them is visible since colors overlap. Remove the largest one and then the whole thing can become a valid compound with no need for tie constraints.

1 Like

This is the way to go.

You can also keep the large one and remove both smaller decks. After compounding, the larger one will be split into two separate faces.

Could you please take a look at this? As you mentioned, the cylinder became a compound, but in this file I sent, it doesn’t work. Thank you in advance. After making it a compound, the mesh cannot be applied.

Indeed, compound creation fails here when applied to all parts at once but you could use it for everything apart from the hull and then connect the two parts with tie constraints. It would be easier if the hull had some surface partitions (edges) where it connects with the other part consisting of the deck and bulkheads.

Thank you very much, you’ve been very helpful. I’m grateful for your interest in my analysis.

I tried fixing your geometry but had no success at all. Usually, compound creation works very well; it is an OpenCascade function, but I cannot figure out why it does not work in your case.