Mechanical event simulation

[pugAA]

Hello,
I'm a student and I have never used Algor before.
I'm trying to model a calandering process and I'm encountering the following problems:
- I can't simulate the rotation of the top cylinder;
- I can't model the surface contact between the parts (when friction contact is assigned, there's no convergence at all).
- When I try to simulate only the press-fit operation (without the rotation of the cylinder) with friction contact I have penetration of the parts.

I hope to clearly explain the problem.

Thanks,

Angelo

Edited by: PugAA on May 31, 2010 12:00 PM Edited by: PugAA on May 31, 2010 12:01 PM

[pugAA]

Here is the .fem file

[John_Holtz]

Hi Angelo,

Unfortunately, the .FEM file is not the complete input. To get the complete model, you should use the "File > Archive" command, and then provide the resulting .ACH file. (Things that are missing are the material properties, all of the surface-to-surface contact definitions, and all of the Analysis > Parameters.)

But I could see enough of the model to make the following suggestions. (I assume that the two smaller cylinders are on the bottom, and the one larger cylinder is on the top.)

1. The top cylinder will not rotate because it is rigidly held in translation in X, Y, Z. In order to "rotate", the nodes need to translate in space. In particular, three points not in a straight line fixed in Tx, Ty, Tz will fully prevent a part from any rigid body motion. (This is not just Finite Element Analysis; this is true of any type of structure.)

One method of holding the top cylinder while allowing it to spin is to use beam elements. See the paragraph "Bonded Contact Between Bricks and Beams" on the page "Autodesk Algor Simulation > Meshing Overview > Mesh Overview > Creating Contact Pairs > Examples of Contact" in the documentation. In your case, you would use a pinned boundary condition in place of the torque that is shown in Figure 3.

2. Since the surface-to-surface contact input is missing, it is difficult to say which input would make the most effect. When penetration occurs, this indicates that a higher contact stiffness is required. (Think of contact as adding springs between the parts. If the springs are too weak, then penetration occurs mathematically.)

Since the analysis parameters input is missing, I do not know how the load is applied. Initiating contact can be difficult to converge, so it can be helpful if the load is ramped slowly until contact occurs, and then the load can be ramped at normal speed.

Also, contact is difficult when the nodes between the contacting bodies match up. I suggest that you put a small space between the parts (1 mm) and mesh the model. Although this does not guarantee that the meshes will not match, it is more likely that the random mesh between disconnected bodies will not match. Then, this gap between the parts can either be "eliminated" by adjusting the surface-to-surface contact tolerance, or by moving the parts at the beginning of the analysis by 2 mm to close the gaps.

A lot of details about surface-to-surface contact is described in the documentation starting on the page "Autodesk Algor Simulation > Setting Up and Performing the Analysis > Setting Up Part 2 > Nonlinear > Loads and Constraints > Surface-to-Surface Contact".


The tutorial under "Help > Tutorials > Analyzing and Evaluating Results Tutorials > Piston Mechanical Event Simulation" may be helpful for several aspects of your work. If you have not gone through it, I highly recommend it.

Sincerely,
John Holtz
Product Design Engineer, Algor Simulation
Autodesk, Inc.

[pugAA]

Hi John,

I tried to follow your suggestions, but I still can't obtain a good model.

In the .ach file you'll see a simplified model.

In reality the bottom cylinders have a translational movement in y-axis

and they can idle rotate.

The top cylinder is the driven one, is fixed in y-axis and gives the

translational movement to the sheet metal thanks to friction contact.

I tried to use contact between beams and bricks as you'll see, but

beams can't keep the cylinder fixed.

Thanks for your support.

Angelo

[John_Holtz]

Angelo,

The top cylinder was missing boundary conditions, so it was free to move. I have added the boundary conditions in the attached archive.

I made some other changes just to optimize the model and speed up the runtime. Naturally, you may need to make further changes to simulate the reality. The changes I made include:

• reducing the number of prescribed displacements on the sheet. (I assume it is being pulled in reality, so putting PDs on the front is more realistic. Perhaps they need to be over the full length on the front.) Applying PDs to the entire sheet is incorrect because that would prevent the sheet from elongating in the X direction.
• I modified the surface attribute of some of the lines on the contacting surface. This reduces the number of contact elements involved in the analysis.

P.S. Change the extension of the attached file from .zip to .ach, and then open it with Algor.

John Holtz

Product Design Engineer, Algor Simulation

Autodesk, Inc.

[pugAA]

Hi John,

I appreciate your suggestions really much, but I need your help again.

In the reality, the metal sheet isn't either pulled or pushed.

The top cylinder has the spin motion (for example 10 RPM) and the metal

sheet advances by friction.

How can I assign this movement to the part?

Angelo

[John_Holtz]

You are 95% of the way there Angelo!

First, change the element type of part 5 from Truss to Beam, and enter the Element Definition data for the beams.

Second, add a prescribe displacement (PD) to one end of the top roll where the boundary condition is. On the PD dialog, set it to be a rotation instead of a translation, and enter the rest of the input as normal. The magnitude can be handled in any number of different ways -- it just depends on how you think. I prefer to enter a magnitude of 1 revolution. Then, the load curve is used to create the rotational speed (in rev/second in your setup). For example, 10 revs in 5 seconds is 2 rev/sec = 120 RPM.

Depending on the real situation, you could add a PD to the opposite end of the roll, too.

[pugAA]

John,

finally the cylinder is rotating.

Thank you for your suggestions!

[pugAA · Accepted solution]

John,

finally the top cylinder is rotating.

Thanks a lot for your suggestions!

[ashwikgreddy]

John,

I was having a similar problem and so i read through ur suggestions. In this model, i see that you did put the boundary conditions for the top cylinder. When i saw the model the spokes were connected from all the surface nodes of the side of a cylinder to a point(centroid) outside the model- how did you create this point outside. When i try to do this all the spokes are coonecting to the center of the side surface and not at a distant point like you did. Please help

[John_Holtz]

Hi,

There are a number of commands that could have been used. The "Mesh > CAD Additions > Joint", or "Setup > Loads > Remote Loads" will create similar structures. I probably used the "Draw > Modify > Point Move" to move the node outside of the model just for clarity. As long as the two boundary conditions are on the centerline, it doesn't make much of a difference where they are along the length.

[ashwikgreddy]

Thanks for the reply John. Here is what am doing. I have a plain cylindrical drum(not completely solid as the above model which u did, it is hollow with x thickness at the wall). I am using MES for this analysis. Did put brick as an element for this drum and with some steel material. Meshed successfully, after this am using centroid locator to create beam spokes on each end of the cylinder connected in the center. Did put nodal boundary condition at the center( no translation condition) on both the sides. Now applied a nodal displacement on one end of the cylinder to rotate at x speed. Am still running the analysis now, but i guess it should run as intended, runs very slow for some reason even though i have only one simple part. Now my question is i want this cylinder drum to be half filled with water and then rotate again - is this possible ? if so how do i do this ?

[ashwikgreddy]

Attached is my part

[S.LI]

Hi,

Several of my comments on your model:

1.) please check-on "large rigid body rotation" for part 2 in element definition -> advanced;

2.) Rotate 60 revolutions. Is this necessary? Results might be floating away due to long-period numerical error accumulations. You have to be very careful on this.

Your model is simulating a kind of light flexible structures. The dynamic response is very complicated. I can see this in simulation results, even without fluid-structure interaction (FSI).

[ashwikgreddy]

I understand now. I was not using a real scenario for rotation, i understand that 60 is too high- i changed to 5 and now running fine and quick. My next question is how do i put water inside this drum and then rotate again. Are fluids possible in MES, how to achieve this. Please help me out with this. Thanks

[John_Holtz]

The answer about the water in the drum depends on what effects you are hoping to capture.

• If you need to see the water splashing (like a washing machine), the answer is no.
• If the speed is slow enough so that the water basically stays at the bottom half, but you need the water for the weight and displacements it creates, the answer is yes. Create a new part representing the water, define the element type to be hydrodynamic, and define surface contact between the surface of the water and the surface of the drum.

Let us know how it goes and when the clothes are clean

[ashwikgreddy]

I created the part but am sure how to put the material as water as it does not have an option in MES for me to put water as a material...sorry if i am missing something

[ashwikgreddy]

sorry i mean to say am not sure how to put water as a material in MES

[ashwikgreddy]

Also my other question was- suppose i apply some surface temperature to outside of the drum and put some temperature to inside the drum liquid. I want to calculate the resultant final temepratures of water as well as drum outside surface, but i dont see anything related to temperature related in MES analysis results. Is this possible ? Sorry am a newbie with this software, so am not sure its capabilities. Thanks

[S.LI]

Please see the attached model. Part 3 is water and Part 4 is the container.