Plate Models: Connect Edges

[scudelari]

Hello Everyone,

I mostly process plate models and I have basically have to simulate connections between parallel plates with Rigd Links. 

I have to get rid of all those inclined lines (such as the selected lines).

I already posted some questions in this forum, such as:

http://forums.autodesk.com/t5/Autodesk-Simulation/Rigid-Link-between-EDGES-Best-way-to-do-it/m-p/322...

http://forums.autodesk.com/t5/Autodesk-Simulation/Automation/m-p/3217904

This is killing me. I am spending like 3 hours a day doing this.

I can see some ways to solve the problem PROGRAMATICALLY:

- Filter the selection of the lines by its direction. There is already a filter that allows you to filter the selection of lines by lenght.

- Create a program to open (hack) the FEM file and remove the lines from a given part that is not on the direction I want.

Both solutions, if one has access to the object that compose the FEM model, are piece of cake.

The problem is that the FEM filetype is binary and there is no InterOp library available for Simulation.

Is there any way to open the FEM files using some library?

Maybe I can could even use some Simulation dll to manage the operations on the FEM file?

If not, what do you guys think about releasing another Tech Preview with the filter I wanted 😛 ? Honestly, a skilled programmer having access to the code could make this filter in 2 hours...

Thanks a lot, guys!

[John_Holtz]

Hi,

I think the real issue is to create a function to do what you need: connect plates together. To do that, we need to know what directions are you locking together with the rigid elements. All directions? Only directions ABC?

Depending on those answers, I wonder if there is another modeling approach that would be easier. For example, could you use plate elements to connects the two plates, and therefore create the link plate in your CAD? (Are you creating the models from CAD or by hand?)

Are the plates (edges) always parallel? If so, then an option on the "Draw > Design > Contact Elements" dialog to create the shortest line would be a solution. The user would not need to do any calculations and enter a minimum and maximum line length to create. If the plates are not parallel, then what direction are the lines?

What if the mesh is different on the two plates? How should the two plates be connected together?

I do not know the scenario, but I can imagine a situation where lines in a radial direction is needed, such as to connect a shaft to a hole when a gap exists between the two. So, whatever needs to be done to control the direction, does it also need to work in cylindrical and/or spherical coordinates?

Would you be opposed to a mathematical solution instead of generating line elements between the parts?

Can you think of other uses for the funtionality to generate lines or a mesh between parts?

OK, the above is work for the future. For the present,

1. Why are you using rigid elements instead of beam elements? Rigid elements require the additional step of placing each one on a separate part number. 😞
2. How are you generating the connecting lines? How did the diagonal lines shown in your image get created?
3. What step in your 3 hour process takes the most time?
4. Are you familiar with "Selection > Subentities" or "Selection > Expand > Chain Border"? If you are using the "Draw > Design > Contact Elements" command, it would be easier to pick the edge ("Selection > Select > Edge") or lines with the chain border, and then "Selection > Subentities > Vertices". If you were to use the "Move or Copy" command, then "Selection > Subentites > Lines" is useful.
5. Do the diagonal lines effect the solution? If the rigid elements connect the two plates in all 6 directions (3 translation+3 rotation), then the diagonals probably do not need to be deleted if you use beam elements instead.

I'm sure there are other things that did not come to mind, but hopefully this gets the brain storming process started/continued.

[S.LI]

For your specific case, I'm not sure if the following way helps or not:

1.) first step: by Selection->Shape->Circle to select all lines around the "connection" region;

2.) second step: to select the inclined line by filter line length, since inclined lines are usually longer than others. By carefully choosing Max and Min length, it could be done, I guess.

[scudelari]

Dear Mr. Holtz,

I really appreciate you taking your time to answer me. I will try to express more clearly what I have to do and then I will answer all the questions you asked.

I am modeling lifting parts for very heavy pressure vessels. The company I work for is specialized in the rigging project for this kind of equipment and one very important part of the job consists on the verification, project and reinforcement of trunnions and lugs.

Naturally, we are using plate elements for the simulation of the equipment’s body.

The rigid links are here used to simulate the weld that holds the plates together.

The image you saw before was of a simulation of a trunnion. The inventor model is attached.

After some investigation, I found out that if I cut the plate under the saddle so that it would have the same shape (I actually create 2 plates and trim them using the same profile in inventor. This guarantees that I have 2 different parts for the mesher), the Mesher creates pretty much the same mesh so that one vertice is right above the other.

NOTE: Both the saddle and its cut “shadow” on the plate are cut by a circular profile, thus cut as a cylinder not a cone.

As you suggested, I do use the Contact Elements functionality having its length limited to generate the lines in a new part. The problem, as you saw, is that, since the body of the equipment and the saddle are curved, the length of the generated lines is not constant. The inclined lines are generated because I have to limit the length till the longest possible. In the vicinity of the longest, only one line is created, but far away from it, several lines are created. The reason for this is that I also need a mesh refined enough. I mean, the refinement of the mesh is about half the distance between the two plates.

The part that contains this line I set as beam and I put everything 1 in the table for the Element Definition. As far as the material goes, I set it to a custom “High Stiffness” material having something like 1E12 N/mm2 as modulus of elasticity (I actually created 4 because some models allow higher stiffness, some allow a lower value. If the warning message appears, I do lower the value).

Since the contacts have about 300 vertices, I have to delete about 200 of them manually – This is the part that takes me hours. Specially because one of the things I have to design is precisely the thickness of the saddle’s plate. If I change it in inventor (I can’t simply change the thickness in Simulation because the distance between the plates also changes – They are modeled to the midplane.), I have to reset everything. The integration between Inventor and Simulation with regard to surfaces has already been discussed here: http://forums.autodesk.com/t5/Autodesk-Simulation/Associativity-between-Inventor-and-Simulation-SURF...

As far as your suggestion of modeling this as a surface in the CAD model, I don’t know if this would bring the same results. I must allow a displacement between neighboring vertices that are on the same plate and – suppose a surface gest meshed to create these lines – it would also connect those vertices. I perceive the same problem if I leave a X connecting the four vertices of two plates. Those vertices won’t have the same freedom as it connected individually.

I can see this functionality being used to connect things as I have to connect here: The length limit put in the Contact Elements function is not enough to generate the desired connection when the mesh is too refined in relation to the distance between the parts.

Of course it would be cool to limit the orientation of the lines radially, but I can see fewer applications for that.

Thanks a lot for the support, and if there is anything I can do, please don’t hesitate.

PS: S. LI: The line filter by length is useless in this case, since the Contact Elements function already has built-in this filter.

[scudelari]

I was thinking about the problem.

Probably if it was added to the Contact Elements function a way to connect the vertices from one set only to the closest vertice to itself in the other set would be easier to implement and would do the trick.

Thanks!

[John_Holtz]

Hi,

Take a look at the attached image "isometric view". If I understand your layout, plate "1" gets welded to plate "2-3" around the perimeter of "2", and plate "2-3" gets welded to the tank around the perimeter of "4".

Assuming this is correct, take a look at the attached image "end view". Imagine that the analysis indicates that the thickness of plate "1" needs to be increased, so to remain technically accurate, the location of the plate elements (at the midplane of the real plate) needs to move outward. The question is, does point "A" move radially outward to point "B", or does the width of the plate remain the same, so point "A" should move straight up to point "C"?

Based on the radius of the tank (large) compared to half the difference in thickness (small), it is probably acceptable to let plate "1" expand from "A" to "B". After all, the accuracy of plate elements is probably worse than the change due to expanding the width of plate "1" from "C" to "B". If all of this is true, then you can

1. Select the lines on plate "1"
2. "Draw > Pattern > Scale or Copy"
3. You want to scale it in 2 cartesian directions, so choose "Perpendicular to..."
4. Set the centerline of the tank for the "Scale direction vector" and "Fixed Point"
5. Calculate the "Scale factor" to go from one radius to the larger radius.
6. Check the box for "Move Ends"
7. Click OK to expand plate 1 and the welds connected to it from point "A" to point "B"

Give it a try.