Problem in contact pair

[Anonymous]

Hello,

I can't obtain realistic friction contact.

I have a top cylinder which has the spin move (0.632RPM).

A metal sheet is supported by two other cylinder that are free to rotate on their axis.

The top cylinder should drag the metal sheet by friction contact.

The problems are:

- The advancement of the metal sheet is not constant and doesn't match with the real value;

- The two bottom cylinder almost can't rotate at all.

Thanks for all suggestions.

I can't attached the file because is too big (8MB)

Angelo

[John_Holtz]

Angelo,

To confirm that the free spinning cylinders are set up correctly, try adding a nodal force in the tangential direction. Does this make the rolls spin?

To simulate a round cylinder, your cylinders would need a fairly fine mesh around the perimeter. For example, imagine that there were only 6 elements around the perimeter. This hexagon would touch the the plate on the corners of the "roll" but not on the flats of the "roll".

Also, check that there is compression in the strip. If the contact tolerance is too small, there may not be enough grip between the driven roll and plate. See the chapter "Autodesk Algor Simulation > Setting Up and Performing the Analysis > Setting Up Part 2 > Nonlinear > Loads and Constraints" in the documentation for help on the contact.

Last thing. I presume you have created an archive of the model ("File > Archive > Create") and that is the 8 MB file that you are trying to attach. If it is too big, you could try this first: delete the files listed in step 5 below, create a new archive, and see if that is small enough. Otherwise, do the following:

1. make three copies of the model.
2. In one copy, delete everything except the top cylinder and plate
3. In second copy, delete everything except the second cylinder
4. In the third copy, delete everything except the third cylinder.
5. In each copy, use My Computer to delete these files from the "model name.ds_data\1\ds.mod" folder:

• elements.dbf
• nodes.dbf
• nodecond.*
• elemcond.*

1. Then make an archive of each of the three models.
2. Post the three archives.

[Anonymous]

Hi John,

The file size is already too big (about 2MB in.zip for any part)

[Anonymous]

Hi, pugAA

A general tip (for anyonelse interested)

www.sendspace.com is a terrific website for uploading medium-sized files. (This is not an ad or anything, it's my personal experience. I hope I'm not breaking any rules?)

[Anonymous]

Hi Bjorn,

thanks for your suggestion.

I don't know if it is possible.

I'll wait for more information.

Regards,

Angelo

[S.LI]

Here is a simple model for frictional contact. Part 3 follows the rotation of part 1.

Please check and compare the contact settings between this model and yours.

Hope it helpful.

[Anonymous]

Hello,

I compared the contact settings and I can't see any difference except

for the friction coefficient.

Here is a .jpg of the model with the main parameters.

I know it's far from send a .ach file but I hope it would be useful for you.

Angelo

[S.LI]

1.) Please make sure nonzero pressures existing between the contact surfaces. This could be easily checked in results. 

2.) Fraction factor is 1, which seems not reasonable to me. This parameter should come from experiments or material manual.

3.) If everything looks OK, results are still not right. I guess you can disable the bottom two cylinders, and constrain the bottom of metal sheet in Y. This will tell us if the metal sheet moves right.

4.) If metal sheet is OK, then you can add the two supports back.

5.) Another method is you can create a 2D model. It should be capable of simulating your problem. Also, the model size will be much much smaller than your current one.

[S.LI]

I think I know the reason why your model is not stable.

As you see in my shared model, parts contact with almost the whole face. So contact pairs balance each other, and the finial average results look OK.

But your model is line contact, (it's point contact in a similar 2D model), which is much more sensitive with mesh and contact settings.

Unfortunately, I don't know how to fix it here.

[John_Holtz]

Angelo,

From looking at the images, it looks like you have a very fine mesh at the center of the three disks. It looks like you did a mesh between two objects, an arc and a line, which created dozens or hundreds of triangular elements at the centerline. You may want to consider making a smaller model (fewer elements) by drawing the complete outline of the parts, each one on a different part number, and using the "2D Mesh" generation to mesh the 4 parts. This will give a more uniform mesh size and eliminate a bulk of the model. (Then extrude the parts like you did before.)

Second, the static friction and dynamic friction should not be the same value. When they are the same, The solution is unstable because it can toggle between a static situation and dynamic situation, and mathemaically, they result in the same "solution". (Or something like that. Maybe it's better to say that the solution doesn't know if it is static or moving because both solutions are identical.) Set the dynamic friction to a smaller value.

Do you have beam elements on the top roll to transmit the torque (the rotational prescribe displacement) into the brick elements? That is a requirement because brick elements do not have the ability to transmit torques/moments. See the documentation (Help > Contents) page "Autodesk Algor Simulation > Meshing Overview > Mesh Overview > Creating Contact Pairs > Examples of Contact" for more details.

[Anonymous]

It's not clear, but the model has beam elements (you may see the three disks in green that isn't the color of the surfaces).

I changed the coefficient of friction. It was exactly 1 because I thought that would prevent slipping between the parts.

I plotted the Y-reaction forces on the top disk in a press-fit simulation (without rotation) and they nearly match the theoretical value. So the forces exchanged by the whole system may be right. Could it be right?

[Anonymous]

Hello again,

Here is the 2-D model. It's still unstable for me.

Thanks for any suggestions.

Regards.

Angelo

[zhuangs]

I got the 2D model sent by John.  The model even cannot be checked.  I would recommend we not waste time on 2D model, which has a lot difference from 3D model for thin sheet.  Please contact the sell representavie to figure out a way to send the model to me.  I may help to make it work.

- Shoubing

[Anonymous]

Hi Zhang,

The 2-D model should work too because the sheet is not thin (135mm).

I don't know any other way to send you the 3D model.

Can you write here your e-mail address?

Regards

Angelo

[zhuangs]

The attachment shows the error when "Check model" for the 2D model you attached.  And there are three "Error" in ds.ldd file.  It seems that the 2D model is not complete or has something wrong.

Anyhow, I think it is a bad idea to simplify your model from 3D to 2D, no matter whether 2D model works or not.

I will figure out how to send the 3D model.  BTW, what is the size of the archieve of 3D model.

[S.LI]

I guess you can use tar in Linux or WinRar in Windows to archive your model into multiple volumes. The size for each volume should be less than 8M or 6M. Then you can upload them piece by piece.

I hope this is allowed here.

[zhuangs]

Please let me know your email address.  And I will send you a FTP.  So you can upload the model archieve of your 3D model there.  This will be much easier for both of us.

[Anonymous]

my e-mail address is: guitarguymad@hotmail.com

Thank you

[zhuangs]

Please create one and only one archieve of the model (model only) via ("File > Archive > Create"), and then upload the archieve via FTP.

[zhuangs]

Hi,

I have two quick questions:

(1) The total duration is 1.2s, but why the load curve 1 is (0.0,0.0)->(1.0,10.0)? I am wondering whether the load curve you want is (0,0.0)->(1.2,10.0) or (0,0.0)->(1.0,10.0)->(1.2,10.0).

(2) The load curve 2 is to control the Y- movement of part 3 and part 4.  I want to know what's the function.  And is it as designed?

-zhuangs