[Workbench] Rope-like behaviour

johannes.karrasch · User Joined: 24 Jan 2014 Posts: 7

Hello everyone,

First of all, I want to excuse for my not perfect English since it isn't my mother tongue.

However, now to my problem, which I'm facing at the moment. As part of my master thesis I have to simulate the application of a fastening device, which I develope during my master thesis. It can be mechanically compared with a pulley problem in it basic concept, but instead of one rope, it uses two ropes, which lie on top of each other. Here is a sketch of the fastening device and the strapping put around it: https://www.dropbox.com/s/v78prd92q7dcgd9/aktuelle_loesung.jpg

Before I modell the whole fastening device, I want to modell just one out of the three poles. It doesn't matter, if I choose the 90Â° or 180Â° setup. I already have a handwritten static mechanical calculation of the whole system, which I want to compare to the simulation. When I use just one rope instead of two and use a pretty stiff material (e.g. steel), I get results which differ just about 1% from the handwritten calculation. However, when I use two ropes, I get completly different results due to the fact, that in the model the friction is applied both ways - from the inner belt to the other belt and the other way round, while in the handwritten calculation only the normal force of the outer belt on the inner belt is taken into account. Sadly I'm really new to Ansys at all and do not know, how to set up the rope-like behaviour to continue this model. Furthermore I seek your advice on the setup of my model.

I just know, that the material is a polyester, I sadly do not have more information. I tried to contact the manufacturer of the fibre and of the belt itself, noone knows the young's-modulus of the belt or the poisson ratio, from which I could make my own material. Due to the fact that polyester (the strapping is most likely from PET-fibers) normally shows an anisotropic behaviour, this gets even more complicated. But I contacted the professor, who does his research in this field of material science at my university, and even he couldn't help me with this material data. He suggested, that I just take into account the material data in direction of the pulling force, which I can determine from the material data sheet of the fiber-producer (young's modulus: 6.76 GPa; max tensile stress: 841.8 MPa).
Here is a screenshot of my Ansys Workbench with the momentarily setup, I use: https://www.dropbox.com/s/4pdw118ne0l3js7/Screenshot%202014-01-09%2014.20.14.png

Here are my questions:

1. How do I model a rope-like behaviour in Workbench? I read something about an APDL-command that could be inserted, however I can't find out, which one I have to use.
2. Is it even possible to model this model in 3D or should I do it in 2D? Since I just know the basics in Workbench, I would like to keep using this programm instead of the Ansys Classic. I would have to learn this programm just like the other one from the start.
3. Is it possible, as I described above, to set the contact friction acting just in one direction (screenshot 2 between the two belts) from the outer belt onto the inner belt, while when I apply a force to the inner belt, there is no friction acting on the outer belt. I want to apply it this way, because that is how the handwritten calculation was done.

Any other hints would be really helpfull too and greatly appreciated!

Thank you in advance!

Johannes

hervandil.santanna · User Joined: 06 Jan 2009 Posts: 116

Hello,

Read in the manual about the element LINK180. Using the correct setup (keyopt 3), you can set this Link (a truss element) to tension only (zero stiffness if compresssed).
Then, in which LINE branch in your geometry create a COMMAND with something similar to this (in each line):

ET,matid,LINK180
!KEYOPT,matid,3,1
SECTYPE,matid,LINK
SECDATA,area

After that, read about the command INISTAT, because you will have to apply an initial strain/stress, otherwise your model will not run.
Best regards

hmsantanna@petrobras.com.br

"johannes.karrasch" ---27/01/2014 15:47:23---Hello everyone, First of all, I want to excuse for my not perfect English since it isn't my mother t

De: "johannes.karrasch" <johannes.karrasch@tu-harburg.de>
Para: xansys@xansys.org,
Data: 27/01/2014 15:47
Assunto: [Xansys] [Workbench] Rope-like behaviour
Enviado por: xansys-bounces@xansys.org

Hello everyone,

First of all, I want to excuse for my not perfect English since it isn't my mother tongue.

However, now to my problem, which I'm facing at the moment. As part of my master thesis I have to simulate the application of a fastening device, which I develope during my master thesis. It can be mechanically compared with a pulley problem in it basic concept, but instead of one rope, it uses two ropes, which lie on top of each other. Here is a sketch of the fastening device and the strapping put around it: https://www.dropbox.com/s/v78prd92q7dcgd9/aktuelle_loesung.jpg

Before I modell the whole fastening device, I want to modell just one out of the three poles. It doesn't matter, if I choose the 90Â° or 180Â° setup. I already have a handwritten static mechanical calculation of the whole system, which I want to compare to the simulation. When I use just one rope instead of two and use a pretty stiff material (e.g. steel), I get results which differ just about 1% from the handwritten calculation. However, when I use two ropes, I get completly different results due to the fact, that in the model the friction is applied both ways - from the inner belt to the other belt and the other way round, while in the handwritten calculation only the normal force of the outer belt on the inner belt is taken into account. Sadly I'm really new to Ansys at all and do not know, how to set up the rope-like behaviour to continue this model. Furthermore I seek your advice on the setup of my model.

I just know, that the material is a polyester, I sadly do not have more information. I tried to contact the manufacturer of the fibre and of the belt itself, noone knows the young's-modulus of the belt or the poisson ratio, from which I could make my own material. Due to the fact that polyester (the strapping is most likely from PET-fibers) normally shows an anisotropic behaviour, this gets even more complicated. But I contacted the professor, who does his research in this field of material science at my university, and even he couldn't help me with this material data. He suggested, that I just take into account the material data in direction of the pulling force, which I can determine from the material data sheet of the fiber-producer (young's modulus: 6.76 GPa; max tensile stress: 841.8 MPa).
Here is a screenshot of my Ansys Workbench with the momentarily setup, I use: https://www.dropbox.com/s/4pdw118ne0l3js7/Screenshot%202014-01-09%2014.20.14.png

Here are my questions:

1. How do I model a rope-like behaviour in Workbench? I read something about an APDL-command that could be inserted, however I can't find out, which one I have to use.
2. Is it even possible to model this model in 3D or should I do it in 2D? Since I just know the basics in Workbench, I would like to keep using this programm instead of the Ansys Classic. I would have to learn this programm just like the other one from the start.
3. Is it possible, as I described above, to set the contact friction acting just in one direction (screenshot 2 between the two belts) from the outer belt onto the inner belt, while when I apply a force to the inner belt, there is no friction acting on the outer belt. I want to apply it this way, because that is how the handwritten calculation was done.

Any other hints would be really helpfull too and greatly appreciated!

Thank you in advance!

Johannes

+-------------------------------------------------------------+
| XANSYS web - www.xansys.org/forum |
| The Online Community for users of ANSYS, Inc. Software |
| Hosted by PADT - www.padtinc.com |
| Send administrative requests to xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+

"O emitente desta mensagem é responsável por seu conteúdo e endereçamento. Cabe ao destinatário cuidar quanto ao tratamento adequado. Sem a devida autorização, a divulgação, a reprodução, a distribuição ou qualquer outra ação em desconformidade com as normas internas do Sistema Petrobras são proibidas e passíveis de sanção disciplinar, cível e criminal."

"The sender of this message is responsible for its content and addressing. The receiver shall take proper care of it. Without due authorization, the publication, reproduction, distribution or the performance of any other action not conforming to Petrobras System internal policies and procedures is forbidden and liable to disciplinary, civil or criminal sanctions."

"El emisor de este mensaje es responsable por su contenido y direccionamiento. Cabe al destinatario darle el tratamiento adecuado. Sin la debida autorización, su divulgación, reproducción, distribución o cualquier otra acción no conforme a las normas internas del Sistema Petrobras están prohibidas y serán pasibles de sanción disciplinaria, civil y penal."

Post generated using Mail2Forum (http://www.mail2forum.com)

johannes.karrasch · User Joined: 24 Jan 2014 Posts: 7

Hey,

Thank you for this quick reply. I will have a look into the manual about this topic.

Does this type element type work with a rectangular cross section area too? I ask, since the cross section are of my belt has a rectangular shape.

Can you explain to me, why I need to apply an initial stress/strain?

Best regards,

Johannes

hervandil.santanna · User Joined: 06 Jan 2009 Posts: 116

Lets try to help.
The LINK180 (and all other link/truss structural elements) have only stiffness in the axial direction. So, no bending effects are expected. For this reason, it doesn't matter the shape of the cross section, just its area value. Moments of inertia are used in beams, that can help bending.
If you don't have a real pre-stress value (something similar to bolt pre-tension), you should apply a tiny strain to stabilize the elements. Remember from the theory that links can rotate one with respect to the other. If you use only one element, this wouldn't be a problem. But probably, to better capture the displacement shape (and values), you will use more than one element in these lines. If you don't constrain the LINKS, you have large displacements. Look for the VM examples concerning this element. Even though, you should run your analysis with large displacements turned on.
Good luck.

hmsantanna@petrobras.com.br

"johannes.karrasch" ---27/01/2014 17:40:18---Hey, Thank you for this quick reply. I will have a look into the manual about this topic.

De: "johannes.karrasch" <johannes.karrasch@tu-harburg.de>
Para: xansys@xansys.org,
Data: 27/01/2014 17:40
Assunto: Re: [Xansys] [Workbench] Rope-like behaviour
Enviado por: xansys-bounces@xansys.org

Hey,

Thank you for this quick reply. I will have a look into the manual about this topic.

Does this type element type work with a rectangular cross section area too? I ask, since the cross section are of my belt has a rectangular shape.

Can you explain to me, why I need to apply an initial stress/strain?

Best regards,

Johannes

hervandil.santanna wrote:

johannes.karrasch · User Joined: 24 Jan 2014 Posts: 7

Hey,

Thank you for your help. I read about the LINK180 and INISTATE command and also understand now, why I need a pre-stress value for the model.

However I still don't know, how to apply the command correctly. As you can see in the second picture of the my first post ( https://www.dropbox.com/s/4pdw118ne0l3js7/Screenshot%202014-01-09%2014.20.14.png EDIT: https://www.dropbox.com/s/cuas9hmzrlpj0q2/Screenshot%202013-12-19%2014.51.59.png 2nd picture of the setup in WB). I have the "Volume bodies" as geometries in ANSYS Workbench. One is the pole and the other two are the inner and outer belt/rope. You said, I have to apply the LINK180-Command to a LINE-body, which I do not have. Can I apply it to the volume element as well? Since I imported the geometry for CAD, I hope, I can still use it or should I redo the whole model in the Model Designer, where I set up all three parts as a line model?

Furthermore can I still use ANSYS WB to do the rest of the modeling then (contact setup, fixed supports etc?)

Sorry, that I seem to bother you guys with real "principable" questions, but this is the first time I use ANSYS at all and I really got stuck on this problem. I took me even a week to find this forum. :/

Thank you for your help in advance! While I wait for your responses, I keep trying to workout how to apply the commands you gave me so far.
Thank you!

Best regards,
Johannes

hervandil.santanna · User Joined: 06 Jan 2009 Posts: 116

Dear Johannes,

I can't open dropbox in my company, so, I can't see any picture.
LINK180 is a line element. You can't replace a volume element (like SOLID186/187) though it.
If you have this possibility, you should think better about your model, and try to convert some volumes to line bodies.
You should read design modeler manual to try it.
Concerning the inistate, look for the VM31 in the manual.
There is a very good example.
Regards

hmsantanna@petrobras.com.br

"johannes.karrasch" ---28/01/2014 18:21:01---Hey, Thank you for your help. I read about the LINK180 and INISTATE command and also understand now,

De: "johannes.karrasch" <johannes.karrasch@tu-harburg.de>
Para: xansys@xansys.org,
Data: 28/01/2014 18:21
Assunto: Re: [Xansys] [Workbench] Rope-like behaviour
Enviado por: xansys-bounces@xansys.org

Hey,

Thank you for your help. I read about the LINK180 and INISTATE command and also understand now, why I need a pre-stress value for the model.

However I still don't know, how to apply the command correctly. As you can see in the second picture of the my first post (https://www.dropbox.com/s/4pdw118ne0l3js7/Screenshot%202014-01-09%2014.20.14.png) I have the "Volume bodies" as geometries in ANSYS Workbench. One is the pole and the other two are the inner and outer belt/rope. You said, I have to apply the LINK180-Command to a LINE-body, which I do not have. Can I apply it to the volume element as well? Since I imported the geometry for CAD, I hope, I can still use it or should I redo the whole model in the Model Designer, where I set up all three parts as a line model?

Furthermore can I still use ANSYS WB to do the rest of the modeling then (contact setup, fixed supports etc?)

Sorry, that I seem to bother you guys with real "principable" questions, but this is the first time I use ANSYS at all and I really got stuck on this problem. I took me even a week to find this forum. :/

Thank you for your help in advance! While I wait for your responses, I keep trying to workout how to apply the commands you gave me so far.
Thank you!

Best regards,
Johannes

+-------------------------------------------------------------+
| XANSYS web - www.xansys.org/forum |
| The Online Community for users of ANSYS, Inc. Software |
| Hosted by PADT - www.padtinc.com |
| Send administrative requests to xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+

"O emitente desta mensagem é responsável por seu conteúdo e endereçamento. Cabe ao destinatário cuidar quanto ao tratamento adequado. Sem a devida autorização, a divulgação, a reprodução, a distribuição ou qualquer outra ação em desconformidade com as normas internas do Sistema Petrobras são proibidas e passíveis de sanção disciplinar, cível e criminal."

"The sender of this message is responsible for its content and addressing. The receiver shall take proper care of it. Without due authorization, the publication, reproduction, distribution or the performance of any other action not conforming to Petrobras System internal policies and procedures is forbidden and liable to disciplinary, civil or criminal sanctions."

"El emisor de este mensaje es responsable por su contenido y direccionamiento. Cabe al destinatario darle el tratamiento adecuado. Sin la debida autorización, su divulgación, reproducción, distribución o cualquier otra acción no conforme a las normas internas del Sistema Petrobras están prohibidas y serán pasibles de sanción disciplinaria, civil y penal."

Post generated using Mail2Forum (http://www.mail2forum.com)

johannes.karrasch · User Joined: 24 Jan 2014 Posts: 7

Hello again,

Sadly, I couldn't advance with my problem. I found the following code in a german ANSYS forum to transfor a line body (beam) into a link180-element.

hervandil.santanna · User Joined: 06 Jan 2009 Posts: 116

Dear mr. Johannes,

That code is correct. When I said you to use "keyopt (3)=1" I was trying to say the value you should assume to this COMMAND. And command is the magic word here. You should check its sintax in manual. And you should see that the sintax is exactly what is put in this code.
Again, LINK180 is a line body element. If you don't apply it to line bodies, it will not work. I have no clue how to model a cable in 3D. So, you should ask your advisor why he insisted in model it in 3D (I can't open pictures from dropbox here in my company. Could you send some pictures directly to my email??)
And concerning the area, check the units. They must be consistent with your model units. For example: if you are using SI, your area obviously should be in m2.
Try to send me some pictures. Or send it to google drive. This I have access.
Regards

hmsantanna@petrobras.com.br

"johannes.karrasch" ---30/01/2014 14:21:15---Hello again, Sadly, I couldn't advance with my problem. I found the following code in a german ANSYS

De: "johannes.karrasch" <johannes.karrasch@tu-harburg.de>
Para: xansys@xansys.org,
Data: 30/01/2014 14:21
Assunto: Re: [Xansys] [Workbench] Rope-like behaviour
Enviado por: xansys-bounces@xansys.org

Hello again,

Sadly, I couldn't advance with my problem. I found the following code in a german ANSYS forum to transfor a line body (beam) into a link180-element.

Code:

/go
esel,s,mat,,matid !choose all elements in the body
!(respect header in
!scriptobject !)
*get,minelem,elem,,num,min !smallest elem nr
*get,ntype,elem,minelem,attr,type !etype of the elements
*get,nreal,elem,minelem,attr,real !RC of the elements

et,ntype,180 !transform beam into rope
KEYOPT,ntype,3,1 !this part I did insert myself, which doesn't work :(
r,nreal,3 !3mm^2 cross section area

alls
/nopr

The code itself works fine, however the part to set Keyopt(3)=1 is missing and all my tries to implement it myself, get me the error:

dean.brown · User Joined: 10 Nov 2008 Posts: 27

Johannes,

You appear to be using Rev13 of Ansys. In that version the tension/compression behavior of LINK180 is controlled by a real constant rather than a keyopt. Try

REAL,ntype,3,,1 ! RC 3=1 sets behavior to tension only

I think it was at Rev15 that control of tension/compression behavior was changed to a key option. Until then the only keyopt was (2), used for cross-section scaling under large deflection analysis.

Best regards,
Dean Brown
Principal Engineer
Microvision, Inc.
USA
www.microvision.com

-----Original Message-----
From: xansys-bounces@xansys.org [mailto:xansys-bounces@xansys.org] On Behalf Of johannes.karrasch
Sent: Thursday, January 30, 2014 8:24 AM
To: xansys@xansys.org
Subject: Re: [Xansys] [Workbench] Rope-like behaviour

Hello again,

Sadly, I couldn't advance with my problem. I found the following code in a german ANSYS forum to transfor a line body (beam) into a link180-element.

Code:

/go
esel,s,mat,,matid !choose all elements in the body
!(respect header in
!scriptobject !)
*get,minelem,elem,,num,min !smallest elem nr
*get,ntype,elem,minelem,attr,type !etype of the elements
*get,nreal,elem,minelem,attr,real !RC of the elements

et,ntype,180 !transform beam into rope
KEYOPT,ntype,3,1 !this part I did insert myself, which doesn't work :(
r,nreal,3 !3mm^2 cross section area

alls
/nopr

The code itself works fine, however the part to set Keyopt(3)=1 is missing and all my tries to implement it myself, get me the error:

edward.carman · Posted: Thu Jan 30, 2014 10:14 am

It was an undocumented change that came in at R14.5 (I remember because I spent a couple of hours trying to track down the reason for suddenly-failing snippets).

dean.brown · User Joined: 10 Nov 2008 Posts: 27

Edward,

Thank you for the clarification. I checked Rev14 and it wasn't changed, whereas it was at Rev15, so I assumed the change was at Rev15, even though it wasn't mentioned in the release notes. I now see it wasn't mentioned in the release notes for Rev14.5 either, although the element documentation was changed. I'll bet that was painful to find.

Best regards,
Dean Brown
Principal Engineer
Microvision, Inc.
USA
www.microvision.com

-----Original Message-----
From: xansys-bounces@xansys.org [mailto:xansys-bounces@xansys.org] On Behalf Of edward.carman
Sent: Thursday, January 30, 2014 9:14 AM
To: xansys@xansys.org
Subject: Re: [Xansys] [Workbench] Rope-like behaviour

It was an undocumented change that came in at R14.5 (I remember because I spent a couple of hours trying to track down the reason for suddenly-failing snippets).

dean.brown wrote:

johannes.karrasch · User Joined: 24 Jan 2014 Posts: 7

johannes.karrasch · User Joined: 24 Jan 2014 Posts: 7

Hey,

It's me again. Sadly I still can't set up the model properly. I had look at the element guide during the weekend and found the SHELL41 element, which has the "cloth" option.

johannes.karrasch · User Joined: 24 Jan 2014 Posts: 7

Hey,

It's me again. I found a promissing model for my problem, which can be found here: http://www.ansys.com/staticassets/ANSYS/staticassets/resourcelibrary/confpaper/2008-Int-ANSYS-Conf-ansys-simulation-flexible-machine-elements.pdf

I have setup a model like this in ANSYS Workbench and my results between handwritten calculation and the solution of ansys differ by about 6.9%. I think, that is a promissing start.

Here are some screenshots from my setup:

I modeled the pole and the inner and outer part of the belt as a SOLID-Element and the membran just as in the example as SHELL-element.

By default ANSYS Workbench uses the right elements, just like the one in the example. But there are still some questions.

At the moment I use as "soft" (low modulus) material PE from the database and for the membran I created my own material, which has the values of a PET-fibre. When I lower the modulus of the PE further, the solution doesn't converge and therefore the calculation is canceled and I receive an error. Furthermore I don't know how to setup the SHELL181 element to "tension-only", since I thought that is done with SHELL41.

In order test the material behaviour I'm modeling a simple beam consisting of the inner and outer layer with a SHELL-element in the middle. Just like I did with LINK 180 element I then want to push and pull it in order to prove, that it is set to "only-tension".

Another thougt was, that I use only the SHELL element, but it seems, that the mixture of SHELL and SOLID seems to be the better choice according to this example. What are your thoughts on this?

I would be really happy, when you could help me with this and appreciate your help!

Thank you!
Best regards,
Johannes Karrasch
_________________
Johannes Karrasch
Engineering Student
Technical University Hamburg-Harburg