Beam Element - Simulate Preload

[travis.potier]

I'm attempting to use a beam element to simulate preload in a tubular component per the instructions in the article linked below.

https://knowledge.autodesk.com/support/inventor-nastran/troubleshooting/caas/sfdcarticles/sfdcarticl...

I'm getting a fatal error E5019 with the description below.

https://help.autodesk.com/view/NINCAD/2021/ENU/?guid=GUID-91754E61-011B-4BFA-B55C-4717672E4C06

My model is a sliver of a tubular component (1/8 degree) with concentric symmetry applied. I'm wondering if the symemtry constraint along with the rigid body connections are causing the over constraint. The beam element line is drawn on the same plane as one of my symmetry planes. Does anyone have any experience and knowledge in this area? Any suggestions are greatly appreciated.

[John_Holtz]

Hi @travis.potier 

I think your suggestion that the symmetry constraint and rigid connector degree of freedom (DOF) are conflicting is correct. Here are a couple of ideas that come to mind:

• If you can remove the DOF from the rigid connector that conflicts with the constraint, that would avoid the error. For example, if the constraint is an X symmetry constraint (TxRyRz), then make the rigid connector TyzRx. Note that this implies that the rigid connector transmits Y and Z forces into the model but no X forces. You need to determine if that is okay.
• Split the model (typically the face) so that the rigid connector and symmetry constraints do not share any nodes.

[travis.potier]

@John_Holtz,

Thanks for the info. I tried your second suggestion above. It cleared most of the errors (I had probably 50+ grid coordinates fail); I now only have 3. The issue I have trying to implement your first suggestion is that I'm using a cylindrical coordinate system to have symmetry about theta. In the choices for degree of freedom on the rigid body, it's only options are x, y, z. Do you have any recommendations on how to handle the degree of freedon in such a case?

Thanks,

Travis

[John_Holtz]

Hi @travis.potier 

I misread your original post. I was thinking "1/8 symmetry" instead of reading it properly. Sorry about that.

You probably have something like this (maybe with a much smaller segment of the full 360 degrees than what I show here). The two faces 1 and 2 have a symmetry constraint in a cylindrical coordinate system. The rigid connector in blue creates a conflict along the red lines where the constraint says to use a cylindrical coordinate system, and the rigid connector says to use a global coordinate system.

I have not tried this, but I wonder if you apply a dummy force to the same surface as the rigid connector, and use the same cylindrical coordinate system for the force, will that force all of the nodes to use the same coordinate system, and will it force the rigid connector to use a cylindrical coordinate system? In the Nastran file itself, the rigid connector does not have a coordinate system associated with it. It just uses the coordinate system assigned to the node. (This is also true for the constraints: the coordinate system gets assigned to the nodes, not to the constraint!) It might work, depending on how the rigid connector is programmed inside the solver.

(edit. added the figure!)

[g.ceruti]

Hi @John_Holtz , the conflict should be only between constraints and rigid connectors with different coordinate systems that invole the same nodes, because both of them try to write a different coordinate system ID in the same nodes Nastran cards "GRID" (in the 7th filed) to define the nodes degree of freedom reference system.

http://help.autodesk.com/view/NSTRN/2019/ENU/?guid=GUID-CCA11D25-0145-42A1-94DC-52226AC8FCD6

While, when you set a coordinate system for a load (force or moment), it writes a coordinate system ID in the FORCE or MOMENT load Nastran cards (in the 4th filed) only to specify the reference system for load components definition.

http://help.autodesk.com/view/NSTRN/2019/ENU/?guid=GUID-7C0E0AB7-1119-4A79-8DC7-8824CD6A3DF0

http://help.autodesk.com/view/NSTRN/2019/ENU/?guid=GUID-2D3F12A0-4823-43CE-BA06-7453BD3B0FB7

[travis.potier]

@John_Holtz,

After more research, I think I'm just totally misusing the tools. I've attached a picture of my model below noting the axis of symmetry and where I inserted the beam element. I'm trying to simulate the magenta part being preloaded into the blue part. I figured it might help if you could see what I was working on.

What I've discovered is that the over constrained nodes aren't the rigid connector nodes; they are nodes at the corners where I cut the part out to insert the beam element (the nodes are on the faces of symmetry about the axis).

A couple of points that I think are problematic are:

• I don't fully understand if it's possible to use a 1-D beam element when the model is such a small sliver with symmetry about an axis being utilized
• I've also attached a screen shot of the beam cross section properties dialog box. According to the dialog box, the beam is turned around the x axis (axis of symmetry). In my part, the y-axis is the axis of symmetry. Would it make a difference if I re-oriented my model so the the axis of symmetry was the x-axis to match the dialog box for the beam properties?

Thanks for all of your input.

[John_Holtz]

Hi @travis.potier 

I do not understand the portion about the conflicting nodes and the coordinate system. Have you figured that out? The faces on the "front" and "back" have symmetry constraints in the hoop direction. What if anything is applied to the two faces where the preloaded beam is being added? Or another way to ask the question is this: how is the preloaded beam connected to the part above and below it? I would have thought that a rigid connector would be used on each of those axial-cut faces. So beam to rigid connector to solid on each end. But of course, the rigid connector attached to the symmetry constraints may create the original problem. 

From the perspective of creating the preload in the beam, the shape, size, and orientation of the beam cross-section does not make a difference. You are just trying to create a load. Use whatever shape is convenient and do not worry about the orientation of the beam or model.

On the other hand, you also want to represent the stiffness of the cut-away part with the beam element. Therefore, the cross-section area of the beam element should be the same as the cross-sectional area of the model. Literally the area of the cut face in the model (1/8 degree you said?). The beam can be a rectangular cross section with dimensions of (1) by (area of the cut face) to keep things simple.

[travis.potier]

@John_Holtz 

I changed the preload element to a bar element with a cross sectional area equal to the cut face. I received the same error message with a couple of nodes being over constrained. I've attached some screenshots showing the nodes that are being report to be being over constrained. As can be seen, they are nodes on the faces of symmetry, not on the beam element.

One thing that may be an issue is that for my rigid body connectors, the dependent entities are edges (the edges between the faces created when I cut the faces in order to get the bar element off of a plane of symmetry). could this be a problem? I'm going to try some modifications to where the dependent entity is a face, not an edge and see what that does.

[John_Holtz]

Hi @travis.potier 

The question is what is assigned to the few nodes with a conflict? What is assigned to the adjacent nodes that do not have a conflict?

I assume the hoop symmetry constraints (in a cylindrical coordinate system) and rigid connector are both using the node shown in the warning message. But what about the next node along the edge? Does it also have the same symmetry constraint and rigid connector? Does it have the same warning?

The attached sample model is as close as I could get to a solution, but clearly some of the nodes on the symmetry face are missing a constraint. (More likely, the constraint is there but acting in the wrong direction.) The setup includes the following features:

1. symmetry constraint in the hoop direction on the near side.
2. symmetry constraint in the hoop direction on the far side.
3. rigid connector only needs to transfer load in the axial direction, so only the axial degree of freedom (X) is set. This is an attempt to avoid a conflict with the hoop constraints.
4. TyzRx constraint on the beam element so that it is statically stable. (Since the rigid connectors are not transmitting forces in the Y or Z direction, the connectors will not provide full stability to the beam.

Model setup

Nodes outline do not stay on symmetry plane

[travis.potier]

@John_Holtz 

Do you have an email address that I can send my model to so that you may be able to see what I have? I've tried to set it up as your model is set up. I must still be missing something as I'm getting the same error messages. I even tried a few different options with no success.

Your help is greatly appreciated.

[John_Holtz · Accepted solution]

Thanks for the model. (I received Travis' model through a support case.) It was my "good" luck that I oriented my test model with the cylinder axis parallel to X, and your "bad" luck that the model is oriented with the axis parallel to the Y axis. When you apply the hoop constraints ("Y" direction = component 2) and the rigid connectors (with TY checked = component 2, to pull in the axial direction), your model has the conflict and gives the error

FATAL ERROR E5019: DEPENDENT MPC AT GRID 433943 COMPONENT 2 IS OVER CONSTRAINED

In other words, the rigid connector (the "MPC") cannot control the Y direction ("COMPONENT 2") because it is constrained by the hoop symmetry ("OVER CONSTRAINED"). 😟

In my example, the hoop constraints (component 2) and rigid connectors (Tx = component 1 in my axial direction) avoid the conflict.

Considering the rigid connector and beam introduce some approximation to begin with, I think the easiest solution is:

1. Split the four (4) surfaces as shown in the image below. You want the new faces beside the rigid connector to be no larger than 1 element tall.
2. The hoop constraints will go on the (4) original faces and will act over 99% of the nodes on the pin part.
3. The rigid connectors can have Ty checked (the axial direction) and Tz checked. Tz direction for the rigid connectors is a good approximation of the hoop direction because your sliver is thin. Leaving Tx unchecked on the rigid connector will allow the nodes to move radially like they should be free to do.
4. The only nodes on the pin part that are not properly constrained in the hoop direction are the midside nodes on the (4) sliver faces between the rigid connector and the hoop symmetry constraints.

P.S. I changed the color of the mesh to yellow to make it stand out better in the image. 

Let us know if that fixes the analysis.

[travis.potier]

@John_Holtz 

I followed your instructions and it appears to have solved the over constraint problem. However, now I can't get convergence.

I'll go ahead and accept the solution and close this one out as my new problem is something entirely different.

Travis