XANSYS Forum Index
    Register    

FAQ    Search    Memberlist    Usergroups    SmartFeedSmartFeed    Profile    Log in
Connect Beam with Solid Elements
 
This forum is locked: you cannot post, reply to, or edit topics.   This topic is locked: you cannot edit posts or make replies.    XANSYS Forum Index -> XANSYS
Author Message
thanos.kontis
User


Joined: 17 Apr 2013
Posts: 6
Location: Thessaloniki

PostPosted: Wed Apr 17, 2013 9:49 pm  Reply with quote

Hello everyone,

I am an undergraduate civil engineering student and for my thesis I have selected to study a historical steel railway truss bridge in fatigue. My first step is to simulate the whole structure using Ansys mechanical. I simulated the steel parts of the bridge using the element BEAM188 and the concrete bridge pedestals using the element SOLID186. My question is, how can I connect these two different kind of elements at the point of the abutments in order to assure full transfer of the forces and moments to the solid element? It's important to mention that in my model I fixed the Degrees of Freedom only on the base of the pedestal and none on the abutment points.

I have read quite a lot about the contact elements and they seem suitable for my problem. As I read from the ANSYS help topics, the use of MPC's seemed capable of connecting beam and solid elements; for every abutment point I created an individual contact element using as a Target element the pedestal and a Source element the appropriate node. Regarding the contact element options, I selected behaviour of contact surface: bonded (always), initial penetration: exclude everything (is that correct??) and the rest on default. However, using the CNCHECK command or "check contact status" I get the following warnings:

- Smoothing on certain contact/target nodes (for example 1130) may have
an accuracy issue. You may switch contact and target surfaces, or
split the current pair into multiple pairs, or use Gauss detection.
MPC will be built internally to handle bonded contact.

- Zero thickness has been found for element 4527 attached to contact
element 6178 (contact element type 23). The influence distance FTOLN
may not be accurate. Please input an absolute value for FTOLN.

When I try to get the solution, obviously I get an error such as "small pivot on node i.e. 50 - check for not sufficiently constrainted model" or there's a huge rotation on a certain node.

I tried other contact elements too, but nothing worked. I hope I'm not making an obvious mistake, but if I am, I'm sorry in advance, since I am newbie and pretty much trying to learn the program by myself using ebooks and the internet.

Thanks a lot
_________________
Thanos Kontis
Undergraduate Civil Engineering Student
Aristotle University of Thessaloniki, Greece
Back to top
View user's profile Send private message
teja.konduri
User


Joined: 09 Apr 2013
Posts: 3

PostPosted: Thu Apr 18, 2013 2:40 am  Reply with quote

Hey,

Are you overlaying your target elements over the solid surface, i.e is your target surface flexible or rigid? Check if there are no gaps between the contact and target surfaces, you can regulate this by using ICONT, to make sure that all your nodes are in initial contact. The use of gauss detection is preferred in order to avoid excessive penetration , you can control this using one of the keyopts..

Teja Konduri
ONET Tech.
France



________________________________

From: xansys-bounces@xansys.org on behalf of thanos.kontis
Sent: Thu 4/18/2013 6:50 AM
To: xansys@xansys.org
Subject: [Xansys] Connect Beam with Solid Elements



Hello everyone,

I am an undergraduate civil engineering student and for my thesis I have selected to study a historical steel railway truss bridge in fatigue. My first step is to simulate the whole structure using Ansys mechanical. I simulated the steel parts of the bridge using the element BEAM188 and the concrete bridge pedestals using the element SOLID186. My question is, how can I connect these two different kind of elements at the point of the abutments in order to assure full transfer of the forces and moments to the solid element? It's important to mention that in my model I fixed the Degrees of Freedom only on the base of the pedestal and none on the abutment points.

I have read quite a lot about the contact elements and they seem suitable for my problem. As I read from the ANSYS help topics, the use of MPC's seemed capable of connecting beam and solid elements; for every abutment point I created an individual contact element using as a Target element the pedestal and a Source element the appropriate node. Regarding the contact element options, I selected behaviour of contact surface: bonded (always), initial penetration: exclude everything (is that correct??) and the rest on default. However, using the CNCHECK command or "check contact status" I get the following warnings:

- Smoothing on certain contact/target nodes (for example 1130) may have
an accuracy issue. You may switch contact and target surfaces, or
split the current pair into multiple pairs, or use Gauss detection.
MPC will be built internally to handle bonded contact.

- Zero thickness has been found for element 4527 attached to contact
element 6178 (contact element type 23). The influence distance FTOLN
may not be accurate. Please input an absolute value for FTOLN.

When I try to get the solution, obviously I get an error such as "small pivot on node i.e. 50 - check for not sufficiently constrainted model" or there's a huge rotation on a certain node.

I tried other contact elements too, but nothing worked. I hope I'm not making an obvious mistake, but if I am, I'm sorry in advance, since I am newbie and pretty much trying to learn the program by myself using ebooks and the internet.

Thanks a lot

------------------------
Thanos Kontis
Undergraduate Civil Engineering Student
Aristotle University of Thessaloniki, Greece






+-------------------------------------------------------------+
| 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 |
+-------------------------------------------------------------+

Post generated using Mail2Forum (http://www.mail2forum.com)
Back to top
View user's profile Send private message
panagiotis.kazantzis
User


Joined: 29 Jun 2009
Posts: 7

PostPosted: Thu Apr 18, 2013 3:40 am  Reply with quote

Hello

You must be carefull when you try to connect beams with solid elements. Beam
elements have 6 degrees of freedom (3 displacements + 3 rotations). Solid
elements have only 3 dof (3 translations) so you can't tranfer any rotation
to the nodes of solid elements. That's why you propably recieve the message
of "unsufficient contraint model". One way to transfer rotations to the
solids elements is to mesh the top surface of solids elements using "rigid"
shell elements. I don't know if you can use contact elements but you must
know that contact elements will lead your analysis in non linear domain and
this will increase the time of your calculation.

Panagiotis Kazantzis
Computer Control Systems SA
Kifisias 94-95
Athens, Greece

-----Αρχικό μήνυμα-----
From: Konduri Teja
Sent: Thursday, April 18, 2013 12:40 PM
To: ANSYS User Discussion List
Subject: Re: [Xansys] Connect Beam with Solid Elements

Hey,

Are you overlaying your target elements over the solid surface, i.e is your
target surface flexible or rigid? Check if there are no gaps between the
contact and target surfaces, you can regulate this by using ICONT, to make
sure that all your nodes are in initial contact. The use of gauss detection
is preferred in order to avoid excessive penetration , you can control this
using one of the keyopts..

Teja Konduri
ONET Tech.
France



________________________________

From: xansys-bounces@xansys.org on behalf of thanos.kontis
Sent: Thu 4/18/2013 6:50 AM
To: xansys@xansys.org
Subject: [Xansys] Connect Beam with Solid Elements



Hello everyone,

I am an undergraduate civil engineering student and for my thesis I have
selected to study a historical steel railway truss bridge in fatigue. My
first step is to simulate the whole structure using Ansys mechanical. I
simulated the steel parts of the bridge using the element BEAM188 and the
concrete bridge pedestals using the element SOLID186. My question is, how
can I connect these two different kind of elements at the point of the
abutments in order to assure full transfer of the forces and moments to the
solid element? It's important to mention that in my model I fixed the
Degrees of Freedom only on the base of the pedestal and none on the abutment
points.

I have read quite a lot about the contact elements and they seem suitable
for my problem. As I read from the ANSYS help topics, the use of MPC's
seemed capable of connecting beam and solid elements; for every abutment
point I created an individual contact element using as a Target element the
pedestal and a Source element the appropriate node. Regarding the contact
element options, I selected behaviour of contact surface: bonded (always),
initial penetration: exclude everything (is that correct??) and the rest on
default. However, using the CNCHECK command or "check contact status" I get
the following warnings:

- Smoothing on certain contact/target nodes (for example 1130) may have
an accuracy issue. You may switch contact and target surfaces, or
split the current pair into multiple pairs, or use Gauss detection.
MPC will be built internally to handle bonded contact.

- Zero thickness has been found for element 4527 attached to contact
element 6178 (contact element type 23). The influence distance FTOLN
may not be accurate. Please input an absolute value for FTOLN.

When I try to get the solution, obviously I get an error such as "small
pivot on node i.e. 50 - check for not sufficiently constrainted model" or
there's a huge rotation on a certain node.

I tried other contact elements too, but nothing worked. I hope I'm not
making an obvious mistake, but if I am, I'm sorry in advance, since I am
newbie and pretty much trying to learn the program by myself using ebooks
and the internet.

Thanks a lot

------------------------
Thanos Kontis
Undergraduate Civil Engineering Student
Aristotle University of Thessaloniki, Greece






+-------------------------------------------------------------+
| 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 |
+-------------------------------------------------------------+









+-------------------------------------------------------------+
| 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 |
+-------------------------------------------------------------+

Post generated using Mail2Forum (http://www.mail2forum.com)
Back to top
View user's profile Send private message
andreas.goumas
User


Joined: 16 Sep 2011
Posts: 55

PostPosted: Thu Apr 18, 2013 4:41 am  Reply with quote

Rolls-Royce Deutschland Ltd & Co KG Sitz/Registered Office: Blankenfelde-Mahlow, Deutschland, Registergericht/Court of Register: Amtsgericht Potsdam, HRA 2731 P,
Persönlich haftende Gesellschafterin/General Partner: Rolls-Royce General Partner Limited, Sitz/Registered Office: Derby, United Kingdom, Register: Registry of Companies Wales and England, 4066556,
Directors/Geschäftsführer: Russel Buxton, Dr. Karsten Mühlenfeld

Confidentiality Notice: This email and any attachments are confidential to the intended recipient and may also be privileged. If you are not the intended recipient please delete it from your system and notify the sender. You should not copy it or use it for any purpose nor disclose or distribute its contents to any other person.

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

Structural Engineer
Rolls-Royce Deutschland Ltd
Back to top
View user's profile Send private message
akbey.kalkan
User


Joined: 11 Apr 2013
Posts: 1

PostPosted: Thu Apr 18, 2013 5:15 am  Reply with quote

Classification: Unclassified / Not Protectively Marked


I would recommend dropping the idea of modelling the abutments all together.

He is trying to do a fatigue assessment of a railway bridge. Just an ordinary constraint with the old school D command will be enough. Trying to model the "whole" bridge with the abutments is just a visual nicety.

First find out the forces in your members and especially those that changes sign while the train travels. Then study the details prone to fatigue with local models as necessary, gusset plates, riveting details etc.

Even local models may not be necessary as bridge codes have charts for classification of details for fatigue but for the sake of training in ANSYS use you can try a few.

Just my thoughts.

--Akbey Kalkan
Babcock



Akbey Kalkan | Senior Analysis Engineer
Babcock International Group
Gilchrist Road | Northbank Industrial Estate | Irlam | Manchester | M44 5AY
mailto:Akbey.Kalkan@babcockinternational.com
www.babcockinternational.com

-----Original Message-----
From: xansys-bounces@xansys.org [mailto:xansys-bounces@xansys.org] On Behalf Of Goumas, Andreas
Sent: 18 April 2013 12:42
To: ANSYS User Discussion List
Subject: Re: [Xansys] Connect Beam with Solid Elements

Hi,
The author stated that he is using MPC always bonded option so the analysis is linear.
I would recommend creating a very simply example and try out the different ways of connecting a solid to a beam, until you are convinced that you have found the correct method. Once you understand, this you can easily model it in your problem.
You can use the MPC approach but you have to select the correct option (Read chapter 9).
You can also use RBE3 command, but again use a test case to make sure you are transferring all forces and moments correctly.
Personally I would use the RBE3 option and would not bother creating contact and target surfaces just to use the "linear" contact option.

Regards,

Andreas Goumas
TS&D Stress (OE-43)

Rolls-Royce Deutschland Ltd. & Co. KG
Eschenweg 11, Dahlewitz, 15827 Blankenfelde-Mahlow, Germany
Tel: +49 (0) 33708 6 3880
Email: andreas.goumas@rolls-royce.com



-----Original Message-----
From: xansys-bounces@xansys.org [mailto:xansys-bounces@xansys.org] On Behalf Of Panagiotis Kazantzis
Sent: Donnerstag, 18. April 2013 12:41
To: ANSYS User Discussion List
Subject: Re: [Xansys] Connect Beam with Solid Elements

Hello

You must be carefull when you try to connect beams with solid elements. Beam elements have 6 degrees of freedom (3 displacements + 3 rotations). Solid elements have only 3 dof (3 translations) so you can't tranfer any rotation to the nodes of solid elements. That's why you propably recieve the message of "unsufficient contraint model". One way to transfer rotations to the solids elements is to mesh the top surface of solids elements using "rigid"
shell elements. I don't know if you can use contact elements but you must know that contact elements will lead your analysis in non linear domain and this will increase the time of your calculation.

Panagiotis Kazantzis
Computer Control Systems SA
Kifisias 94-95
Athens, Greece

----- -----
From: Konduri Teja
Sent: Thursday, April 18, 2013 12:40 PM
To: ANSYS User Discussion List
Subject: Re: [Xansys] Connect Beam with Solid Elements

Hey,

Are you overlaying your target elements over the solid surface, i.e is your target surface flexible or rigid? Check if there are no gaps between the contact and target surfaces, you can regulate this by using ICONT, to make sure that all your nodes are in initial contact. The use of gauss detection is preferred in order to avoid excessive penetration , you can control this using one of the keyopts..

Teja Konduri
ONET Tech.
France



________________________________

From: xansys-bounces@xansys.org on behalf of thanos.kontis
Sent: Thu 4/18/2013 6:50 AM
To: xansys@xansys.org
Subject: [Xansys] Connect Beam with Solid Elements



Hello everyone,

I am an undergraduate civil engineering student and for my thesis I have selected to study a historical steel railway truss bridge in fatigue. My first step is to simulate the whole structure using Ansys mechanical. I simulated the steel parts of the bridge using the element BEAM188 and the concrete bridge pedestals using the element SOLID186. My question is, how can I connect these two different kind of elements at the point of the abutments in order to assure full transfer of the forces and moments to the solid element? It's important to mention that in my model I fixed the Degrees of Freedom only on the base of the pedestal and none on the abutment points.

I have read quite a lot about the contact elements and they seem suitable for my problem. As I read from the ANSYS help topics, the use of MPC's seemed capable of connecting beam and solid elements; for every abutment point I created an individual contact element using as a Target element the pedestal and a Source element the appropriate node. Regarding the contact element options, I selected behaviour of contact surface: bonded (always), initial penetration: exclude everything (is that correct??) and the rest on default. However, using the CNCHECK command or "check contact status" I get the following warnings:

- Smoothing on certain contact/target nodes (for example 1130) may have an accuracy issue. You may switch contact and target surfaces, or split the current pair into multiple pairs, or use Gauss detection.
MPC will be built internally to handle bonded contact.

- Zero thickness has been found for element 4527 attached to contact element 6178 (contact element type 23). The influence distance FTOLN may not be accurate. Please input an absolute value for FTOLN.

When I try to get the solution, obviously I get an error such as "small pivot on node i.e. 50 - check for not sufficiently constrainted model" or there's a huge rotation on a certain node.

I tried other contact elements too, but nothing worked. I hope I'm not making an obvious mistake, but if I am, I'm sorry in advance, since I am newbie and pretty much trying to learn the program by myself using ebooks and the internet.

Thanks a lot

------------------------
Thanos Kontis
Undergraduate Civil Engineering Student
Aristotle University of Thessaloniki, Greece






+-------------------------------------------------------------+
| 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 |
+-------------------------------------------------------------+









+-------------------------------------------------------------+
| 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 |
+-------------------------------------------------------------+


+-------------------------------------------------------------+
| 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 |
+-------------------------------------------------------------+



________________________________

This electronic mail message, including any attachments, is a confidential communication exclusively between Babcock International Group PLC and the intended recipient(s) indicated as the addressee(s). It contains information which is private and may be proprietary or covered by legal professional privilege. If you receive this message in any form and you are not the intended recipient you must not review, use, disclose or disseminate it. We would be grateful if you could contact the sender upon receipt and in any event you should destroy this message without delay. Anything contained in this message that is not connected with the business of Babcock International Group PLC is neither endorsed by nor is the liability of this company.

Babcock International Group PLC.

Telephone: +44(0)20 7355 5300
Fax: +44(0)20 7355 5360
Website: www.babcockinternational.com
Registered in: England and Wales
Registration No: 2342138
Registered Office: 33 Wigmore Street, London, W1 1QX, England

Post generated using Mail2Forum (http://www.mail2forum.com)
Back to top
View user's profile Send private message
thanos.kontis
User


Joined: 17 Apr 2013
Posts: 6
Location: Thessaloniki

PostPosted: Fri Apr 26, 2013 1:45 am  Reply with quote

Hello again,

After some days trying to work out the problem I finally found a solution. Turns out that the MPC solution was correct, it only needed some adjustments.

The "Smoothing on certain contact/target nodes may have
an accuracy issue" problem was solved by changing the contact normals to normal from contact nodes.

Regarding "the Zero thickness [....] The influence distance FTOLN may not be accurate. Please input an absolute value for FTOLN." , I put a negative value on the penetration tolerance factor (FTOLN) (which, as I read on the manual, it fully allows the penetration) and at the same time I excluded all penetration from the calculation. I also clicked the "close gap" option on the contact adjustment to avoide any possible errors then.

All that applied for each individual abutment. Finally the program gave a solution error-free.

Thanks al lot for your help and suggestions
_________________
Thanos Kontis
Undergraduate Civil Engineering Student
Aristotle University of Thessaloniki, Greece
Back to top
View user's profile Send private message
Display posts from previous:   
This forum is locked: you cannot post, reply to, or edit topics.   This topic is locked: you cannot edit posts or make replies.    XANSYS Forum Index -> XANSYS
All times are GMT - 7 Hours
Page 1 of 1

 
Jump to:  
You cannot post new topics in this forum
You cannot reply to topics in this forum
You cannot edit your posts in this forum
You cannot delete your posts in this forum
You cannot vote in polls in this forum
You cannot attach files in this forum
You cannot download files in this forum


Powered by phpBB © 2001, 2005 phpBB Group

sleek template created by Andrew Charron