XANSYS Forum Index
    Register    

FAQ    Search    Memberlist    Usergroups    SmartFeedSmartFeed    Profile    Log in
[APDL] Compression only springs
 
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
razmik.martirosyan
User


Joined: 17 Jun 2014
Posts: 43

PostPosted: Fri Jan 16, 2015 9:29 am  Reply with quote

Hi Everyone,

I am modeling concrete slab-soil interaction and it seems to be logical if I put spring elements under concrete slab soI am wondering if there is a way to model compression only springs in ANSYS?

I.e. the springs should not work in tension as in case of upward of downward curling the parts of slab may be separated from soil freely.

Best Regards
Razmik Martirosyan
Universitat Polytachnica de Catalunya
Back to top
View user's profile Send private message
matt.sutton
User


Joined: 21 Oct 2008
Posts: 134

PostPosted: Fri Jan 16, 2015 10:25 am  Reply with quote

Razmik,
You probably want to search for "contact" in the manual.
Regards,
Matt Sutton
www.padtinc.con


-----Original Message-----
From: Xansys [mailto:xansys-bounces@xansys.org] On Behalf Of razmik.martirosyan
Sent: Friday, January 16, 2015 9:29 AM
To: xansys@xansys.org
Subject: [Xansys] [APDL] Compression only springs

Hi Everyone,

I am modeling concrete slab-soil interaction and it seems to be logical if I put spring elements under concrete slab soI am wondering if there is a way to model compression only springs in ANSYS?

I.e. the springs should not work in tension as in case of upward of downward curling the parts of slab may be separated from soil freely.

Best Regards
Razmik Martirosyan
Universitat Polytachnica de Catalunya






+-------------------------------------------------------------+
| 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
Martin Liddle
User


Joined: 15 Aug 2008
Posts: 1274
Location: Chesterfield, UK

PostPosted: Fri Jan 16, 2015 10:41 am  Reply with quote

On 16/01/2015 16:29, razmik.martirosyan wrote:
Quote:
I am modeling concrete slab-soil interaction and it seems to be logical if I put spring elements under concrete slab soI am wondering if there is a way to model compression only springs in ANSYS?

I.e. the springs should not work in tension as in case of upward of downward curling the parts of slab may be separated from soil freely.
Not exactly what you want but SURF154 will supply foundation stiffness
with real constant EFS.

--
Martin Liddle, Tynemouth Computer Services,
Chesterfield, Derbyshire, UK.
www.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)
_________________
Martin Liddle, Tynemouth Computer Services,
Chesterfield, UK.
Back to top
View user's profile Send private message Visit poster's website
Martin Liddle
User


Joined: 15 Aug 2008
Posts: 1274
Location: Chesterfield, UK

PostPosted: Fri Jan 16, 2015 10:43 am  Reply with quote

On 16/01/2015 17:25, Matt Sutton wrote:
Quote:
You probably want to search for "contact" in the manual.
True Matt but if you look back a few posts Razmick posted a question
about an ANSYS crash when using contact elements and changing material
properties.

--
Martin Liddle, Tynemouth Computer Services,
Chesterfield, Derbyshire, UK.
www.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)
_________________
Martin Liddle, Tynemouth Computer Services,
Chesterfield, UK.
Back to top
View user's profile Send private message Visit poster's website
matt.sutton
User


Joined: 21 Oct 2008
Posts: 134

PostPosted: Sat Jan 17, 2015 8:12 am  Reply with quote

Ah, I see. I'm aware of the compression only springs, but from my quick glance at his description it sounded like contact was what he was after.
Matt Sutton
www.padtinc.com


-----Original Message-----
From: Xansys [mailto:xansys-bounces@xansys.org] On Behalf Of Martin Liddle
Sent: Friday, January 16, 2015 10:44 AM
To: xansys@xansys.org
Subject: Re: [Xansys] [APDL] Compression only springs

On 16/01/2015 17:25, Matt Sutton wrote:
Quote:
You probably want to search for "contact" in the manual.
True Matt but if you look back a few posts Razmick posted a question about an ANSYS crash when using contact elements and changing material properties.

--
Martin Liddle, Tynemouth Computer Services, Chesterfield, Derbyshire, UK.
www.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 |
+-------------------------------------------------------------+

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


Joined: 15 Aug 2008
Posts: 1274
Location: Chesterfield, UK

PostPosted: Sat Jan 17, 2015 3:54 pm  Reply with quote

On 17/01/2015 15:10, Matt Sutton wrote:
Quote:
Ah, I see. I'm aware of the compression only springs, but from my quick glance at his description it sounded like contact was what he was after.

Oh I agree that contact is the correct solution but sometimes if you hit
a problem that you just can't solve then to make progress you have to
find a less satisfactory workaround which is what I was suggesting. The
real solution would be to understand the cause of the SIG$SEGV when
changing material properties with contact elements present.

--
Martin Liddle, Tynemouth Computer Services,
Chesterfield, Derbyshire, UK.
www.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)
_________________
Martin Liddle, Tynemouth Computer Services,
Chesterfield, UK.
Back to top
View user's profile Send private message Visit poster's website
Winfried Schepers
Guest





PostPosted: Sat Jan 17, 2015 4:16 pm  Reply with quote

Quote:
I am modeling concrete slab-soil interaction and it seems to be logical
if I put spring elements under concrete slab soI am wondering if there
is a way to model compression only springs in ANSYS?

I.e. the springs should not work in tension as in case of upward of
downward curling the parts of slab may be separated from soil freely.

since a Winkler foundation is usually a rather crude approximation of a half-space anyway, because it completely neglects soil-structure interaction, a possibly reasonable approach is to use COMBIN39 nonlinear elastic springs, applying the full compression foundation stiffness, but only a small portion of it, say 1/1000, for tension. To avoid numerical issues near the compression-tension transition, you might have to smooth the transition in the force-deflection curve at zero soil pressure somewhat. Each single spring stiffness will depend on the size of the slab elements connected to the spring, but a few lines of APDL are sufficient to apply different stiffness coefficients at each single spring.

With best regards,

Winfried Schepers

------------------------------------------------------------
Dr. Winfried SCHEPERS
mail: schepers@gudconsult.de
Phone +49 30 789089-806
------------------------------------------------------------

GuD Geotechnik und Dynamik Consult GmbH
Darwinstrasse 13
10589 Berlin
Germany



Quote:
-----Original Message-----
From: Xansys [mailto:xansys-bounces@xansys.org] On Behalf Of
razmik.martirosyan
Sent: 16 January, 2015 17:29
To: xansys@xansys.org
Subject: [Xansys] [APDL] Compression only springs

Hi Everyone,

I am modeling concrete slab-soil interaction and it seems to be logical
if I put spring elements under concrete slab soI am wondering if there
is a way to model compression only springs in ANSYS?

I.e. the springs should not work in tension as in case of upward of
downward curling the parts of slab may be separated from soil freely.

Best Regards
Razmik Martirosyan
Universitat Polytachnica de Catalunya






+-------------------------------------------------------------+
| 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
sai.pai
User


Joined: 08 Jul 2013
Posts: 2

PostPosted: Mon Jan 19, 2015 3:33 am  Reply with quote

Hi Ramzik,

To model compression-only springs in ANSYS, you can use the COMBIN39 non-linear springs with tension-only behaviour. Then you can reverse the node ordering so that the relative displacement between the nodes for compression behaviour is positive, which ANSYS will read as tension.

I am not an ANSYS expert and this is something that was suggested to me in this forum when I had asked a similar question. Hope it helps.

Regards,

Sai Ganesh S Pai
Department of Civil Engineering
UBC, Vancouver

________________________________________
From: Xansys [xansys-bounces@xansys.org] on behalf of razmik.martirosyan [razmik.martirosyan@estudiant.upc.edu]
Sent: January-16-15 8:29 AM
To: xansys@xansys.org
Subject: [Xansys] [APDL] Compression only springs

Hi Everyone,

I am modeling concrete slab-soil interaction and it seems to be logical if I put spring elements under concrete slab soI am wondering if there is a way to model compression only springs in ANSYS?

I.e. the springs should not work in tension as in case of upward of downward curling the parts of slab may be separated from soil freely.

Best Regards
Razmik Martirosyan
Universitat Polytachnica de Catalunya






+-------------------------------------------------------------+
| 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
razmik.martirosyan
User


Joined: 17 Jun 2014
Posts: 43

PostPosted: Mon Jan 19, 2015 5:38 am  Reply with quote

Martin Liddle wrote:
On 17/01/2015 15:10, Matt Sutton wrote:
Quote:
Ah, I see. I'm aware of the compression only springs, but from my quick glance at his description it sounded like contact was what he was after.

Oh I agree that contact is the correct solution but sometimes if you hit
a problem that you just can't solve then to make progress you have to
find a less satisfactory workaround which is what I was suggesting. The
real solution would be to understand the cause of the SIG$SEGV when
changing material properties with contact elements present.

--
Martin Liddle, Tynemouth Computer Services,
Chesterfield, Derbyshire, UK.
www.tynecomp.co.uk


Hi Martin, Matt,

Thank you very much for yout responses.

For each time step I was changing material types for each element in my mesh, and giving new properties, the use of contact elements was bringing to errors. Then, before each SOLVE command I am chaging material types to the initial one (with already updated properties) and now this approach works.
Now it seems that the upper layer is not affecting the base in terms of stresses which is strange(i.e. no stresses appearing in subbase) and another problem is adding self weight for upper layer by ACEL (gravity 9.8065 m/s2 = 127092240 m/h2 which brings me another error).

WHat do you think of using LINK180 element as it has only compression behaviour?

Best Regards
Razmik Martirosyan
Universitat Polytachnica de Catalunya
Back to top
View user's profile Send private message
razmik.martirosyan
User


Joined: 17 Jun 2014
Posts: 43

PostPosted: Mon Jan 19, 2015 6:00 am  Reply with quote

Quote:

since a Winkler foundation is usually a rather crude approximation of a half-space anyway, because it completely neglects soil-structure interaction, a possibly reasonable approach is to use COMBIN39 nonlinear elastic springs, applying the full compression foundation stiffness, but only a small portion of it, say 1/1000, for tension. To avoid numerical issues near the compression-tension transition, you might have to smooth the transition in the force-deflection curve at zero soil pressure somewhat. Each single spring stiffness will depend on the size of the slab elements connected to the spring, but a few lines of APDL are sufficient to apply different stiffness coefficients at each single spring.

With best regards,

Winfried Schepers
------------------------------------------------------------
Dr. Winfried SCHEPERS
mail: schepers@gudconsult.de
Phone +49 30 789089-806
------------------------------------------------------------
GuD Geotechnik und Dynamik Consult GmbH
Darwinstrasse 13
10589 Berlin
Germany



Hi Winfried,

Thank you for your response, but to be honest I am not sure how to apply
the full compression foundation stiffness with only a small portion of tension.
It would be perfect if you explain in more details?

Quote:
To model compression-only springs in ANSYS, you can use the COMBIN39 non-linear springs with tension-only behaviour. Then you can reverse the node ordering so that the relative displacement between the nodes for compression behaviour is positive, which ANSYS will read as tension.

I am not an ANSYS expert and this is something that was suggested to me in this forum when I had asked a similar question. Hope it helps.



Hi Sai,

Thank you also for your time and response, but at leasts for now the idea is not the calculation of the stresses appearing in subbase but in the slab so I think its not the best way of do it. Have you used LINK180 element with only compression option?

Best Regards
Razmik Martirosyan
Universitat Polytachnica de Catalunya
Back to top
View user's profile Send private message
Martin Liddle
User


Joined: 15 Aug 2008
Posts: 1274
Location: Chesterfield, UK

PostPosted: Mon Jan 19, 2015 6:12 am  Reply with quote

On 19/01/2015 12:38, razmik.martirosyan wrote:
Quote:
For each time step I was changing material types for each element in my mesh, and giving new properties, the use of contact elements was bringing to errors. Then, before each SOLVE command I am chaging material types to the initial one (with already updated properties) and now this approach works.
Good.
Quote:
Now it seems that the upper layer is not affecting the base in terms of stresses which is strange(i.e. no stresses appearing in subbase) and another problem is adding self weight for upper layer by ACEL (gravity 9.8065 m/s2 = 127092240 m/h2 which brings me another error).
At the risk of stating the obvious, do you have density defined and in
the correct units. Is your unit system consistent because defining
acceleration in m/h2 would be unusual.
Quote:
WHat do you think of using LINK180 element as it has only compression behaviour?
I think it will work just fine but personally I would suggest sticking
with your contact element approach for a bit longer as it may be the
easiest way.

--
Martin Liddle, Tynemouth Computer Services,
Chesterfield, Derbyshire, UK.
www.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)
_________________
Martin Liddle, Tynemouth Computer Services,
Chesterfield, UK.
Back to top
View user's profile Send private message Visit poster's website
razmik.martirosyan
User


Joined: 17 Jun 2014
Posts: 43

PostPosted: Mon Jan 19, 2015 7:17 am  Reply with quote

[quote]
Quote:
Now it seems that the upper layer is not affecting the base in terms of stresses which is strange(i.e. no stresses appearing in subbase) and another problem is adding self weight for upper layer by ACEL (gravity 9.8065 m/s2 = 127092240 m/h2 which brings me another error).

At the risk of stating the obvious, do you have density defined and in
the correct units. Is your unit system consistent because defining
acceleration in m/h2 would be unusual.


Thanks Martin,

I am using simulation time in hours i.e. all the units are in hours not seconds, time also changing by hours ( one hour for eah time step, from 1 to final_time) that is why I was considering that this unit also should be in hours. Please correct me if I am wrong.

Best Regards
Razmik Martirosyan
Universitat Polytachnica de Catalunya
Back to top
View user's profile Send private message
winfried.schepers
User


Joined: 21 Oct 2008
Posts: 43

PostPosted: Mon Jan 19, 2015 7:27 am  Reply with quote

Hi Razmik,

have a look at the documentation of COMBIN39 in the theory manual and the element reference manual. Essentially, while with COMBIN14 the spring stiffness is defined as a straight infinite line in the first and third quadrant of the Force-Deflection plain, with COMBIN39 that curve becomes a piecewise linear polygon. That´s all. Say your peak vertical slab displacements are smaller than 1 m, and the spring stiffness is 1 N/m, then your force-displacement curve might be as follows:

(-10,-10),(0,0),(10,0.1)

As Sai suggested you can also use COMBIN39 with keyopt(2)=1 (tension only), but then the location of your spring nodes must be chosen counter-intuitively.

Alternatively, you can of course use COMBIN40 with FSLIDE<0, or LINK180 in compression only. The results are not supposed to be significantly different, as long as you choose the keyoptions appropriately.

However, as Martin suggested it might be a better idea to stick to the contact approach with SURF154 and EFS. That would be true if your slab mesh is irregular. In that case the spring stiffnesses depend on the size of the elements attached to each spring, and you need different real sets for each spring element, while SURF154+EFS account for that automatically.



Winfried Schepers

------------------------------------------------------------
Dr.-Ing. Winfried Schepers
mail: schepers@gudconsult.de
Tel. 030/789089-806
------------------------------------------------------------

GuD Geotechnik und Dynamik Consult GmbH
Darwinstraße 13
10589 Berlin

Quote:
Thank you for your response, but to be honest I am not sure how to
apply
the full compression foundation stiffness with only a small portion of
tension.
It would be perfect if you explain in more details?


Quote:
To model compression-only springs in ANSYS, you can use the COMBIN39
non-linear springs with tension-only behaviour. Then you can reverse
the node ordering so that the relative displacement between the nodes
for compression behaviour is positive, which ANSYS will read as
tension.
Quote:

I am not an ANSYS expert and this is something that was suggested to
me in this forum when I had asked a similar question. Hope it helps.


Hi Sai,

Thank you also for your time and response, but at leasts for now the
idea is not the calculation of the stresses appearing in subbase but in
the slab so I think its not the best way of do it. Have you used
LINK180 element with only compression option?

Best Regards
Razmik Martirosyan
Universitat Polytachnica de Catalunya






+-------------------------------------------------------------+
| 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
carl.mally
User


Joined: 21 Oct 2008
Posts: 120

PostPosted: Mon Jan 19, 2015 7:42 am  Reply with quote

Quote:
Quote:
I am using simulation time in hours i.e. all the units are in hours not seconds, time also changing by hours ( one hour for eah time step, from 1 to final_time) that is why I was considering that this unit also should be in hours. Please correct me if I am wrong.<<

Maintaining consistent units could become something out of your worst nightmares. For example any time newtons or pascals are applied then seconds are included in the definition unless you make allowances.


Carl Mally
Product Development Engineer
Centro Inc.
950 North Bend Drive
North Liberty, IA 52317


+-------------------------------------------------------------+
| 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
Martin Liddle
User


Joined: 15 Aug 2008
Posts: 1274
Location: Chesterfield, UK

PostPosted: Mon Jan 19, 2015 8:19 am  Reply with quote

On 19/01/2015 14:17, razmik.martirosyan wrote:
Quote:
I am using simulation time in hours i.e. all the units are in hours not seconds, time also changing by hours ( one hour for eah time step, from 1 to final_time) that is why I was considering that this unit also should be in hours. Please correct me if I am wrong.

So what units is your density in?

--
Martin Liddle, Tynemouth Computer Services,
Chesterfield, Derbyshire, UK.
www.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)
_________________
Martin Liddle, Tynemouth Computer Services,
Chesterfield, UK.
Back to top
View user's profile Send private message Visit poster's website
razmik.martirosyan
User


Joined: 17 Jun 2014
Posts: 43

PostPosted: Tue Jan 20, 2015 3:04 am  Reply with quote

Thanks Winfried, Carl


Quote:

So what units is your density in?


Martin, my units for density are in kg/m3.

Best Regards
Razmik Martirosyan
Universitat Polytachnica de Catalunya
Back to top
View user's profile Send private message
Martin Liddle
User


Joined: 15 Aug 2008
Posts: 1274
Location: Chesterfield, UK

PostPosted: Tue Jan 20, 2015 3:59 am  Reply with quote

On 20/01/2015 10:04, razmik.martirosyan wrote:
Quote:
Quote:
So what units is your density in?



Martin, my units for density are in kg/m3.
You either need to change your density unit or your time unit;
personally I would stay in an MKS unit system and change time to seconds
and acceleration to m/s2.

--
Martin Liddle, Tynemouth Computer Services,
Chesterfield, Derbyshire, UK.
www.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)
_________________
Martin Liddle, Tynemouth Computer Services,
Chesterfield, UK.
Back to top
View user's profile Send private message Visit poster's website
christopher.wright
User


Joined: 17 Jun 2009
Posts: 927

PostPosted: Tue Jan 20, 2015 1:32 pm  Reply with quote

On Jan 20, 2015, at 4:04 AM, razmik.martirosyan wrote:

Quote:
Martin, my units for density are in kg/m3.

Now form the quotient (elastic modulus/density) and tell us what
those units are. The quotient will have the dimension length^2/
time^2. if the units aren't meters and hours your problem isn't
dimensionally consistent with a time input in hours. That's good
practice for any mechanical problem, particular with metric input
where you may have used model geometry in mm or cm and physical
quantities expressed in terms of some other length units.


Christopher Wright P.E. |"They couldn't hit an elephant at
chrisw@skypoint.com | this distance" (last words of Gen.
.......................................| John Sedgwick, Spotsylvania
1864)
http://www.skypoint.com/members/chrisw/



+-------------------------------------------------------------+
| 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
lucas.rodriguez
User


Joined: 24 Sep 2011
Posts: 6

PostPosted: Mon Jan 26, 2015 3:08 am  Reply with quote

Dear Razmik,

I suggest having a look at LINK10 elements (Keyopt 3 set as 1,
only-compression). This element is undocumented in last versions of
ANSYS so you will need to check ANSYS 12.0 Help Reference or previous.

For a regular mesh on your slab you may go through with an unique real
constant set. If not, you may need to code an APDL script to find out
the tributary area of each node to assign a more accurate value of
Link-10 input area.

I hope it helps.

Un saludo /Best regards

----------------------------------------

Lucas Rodríguez Velasco

lucas.rodriguez.velasco@alumnos.upm.es

PHD Candidate - ETSI Navales Universidad Politécnica de Madrid

El 2015-01-20 21:32, Christopher Wright escribió:

Quote:
On Jan 20, 2015, at 4:04 AM, razmik.martirosyan wrote:

Quote:
Martin, my units for density are in kg/m3.

Now form the quotient (elastic modulus/density) and tell us what
those units are. The quotient will have the dimension length^2/
time^2. if the units aren't meters and hours your problem isn't
dimensionally consistent with a time input in hours. That's good
practice for any mechanical problem, particular with metric input
where you may have used model geometry in mm or cm and physical
quantities expressed in terms of some other length units.

Christopher Wright P.E. |"They couldn't hit an elephant at
chrisw@skypoint.com | this distance" (last words of Gen.
.......................................| John Sedgwick, Spotsylvania
1864)
http://www.skypoint.com/members/chrisw/ [1]

+-------------------------------------------------------------+
| XANSYS web - www.xansys.org/forum [2] |
| The Online Community for users of ANSYS, Inc. Software |
| Hosted by PADT - www.padtinc.com [3] |
| Send administrative requests to xansys-mod@tynecomp.co.uk |
+-------------------------------------------------------------+


Links:
------
[1] http://www.skypoint.com/members/chrisw/
[2] http://www.xansys.org/forum
[3] http://www.padtinc.com
+-------------------------------------------------------------+
| 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
razmik.martirosyan
User


Joined: 17 Jun 2014
Posts: 43

PostPosted: Thu Jan 29, 2015 4:21 am  Reply with quote

Quote:

You either need to change your density unit or your time unit;
personally I would stay in an MKS unit system and change time to seconds
and acceleration to m/s2.


Dear Martin, the problem here is I have three different models and there are a lot of parameters and calculations done, so if I have to change time unit I might really have a lots of problems.

What would be suggested change in density units?

Quote:

Now form the quotient (elastic modulus/density) and tell us what
those units are. The quotient will have the dimension length^2/
time^2. if the units aren't meters and hours your problem isn't
dimensionally consistent with a time input in hours. That's good
practice for any mechanical problem, particular with metric input
where you may have used model geometry in mm or cm and physical
quantities expressed in terms of some other length units.


Thanks Christopher, in other words are you also suggesting to change the density unit?



lucas.rodriguez wrote:
Dear Razmik,

I suggest having a look at LINK10 elements (Keyopt 3 set as 1,
only-compression). This element is undocumented in last versions of
ANSYS so you will need to check ANSYS 12.0 Help Reference or previous.

For a regular mesh on your slab you may go through with an unique real
constant set. If not, you may need to code an APDL script to find out
the tributary area of each node to assign a more accurate value of
Link-10 input area.

I hope it helps.

Un saludo /Best regards
----------------------------------------
Lucas Rodríguez Velasco
lucas.rodriguez.velasco@alumnos.upm.es
PHD Candidate - ETSI Navales Universidad Politécnica de Madrid


Dear Lucas,

I was really looking this element in Help reference but was not able to find. I will try
to do it in older versions of help. But one more quesion, as my mesh is rectangular,for the simulation only compression soil, should I add only one element from each node of the subsurface nodes and if the size of the element in this case matter?

Thanks all of you for your time and answers!

Best Regards
Razmik Martirosyan
Universitat Polytechnica de Catalunya
Back to top
View user's profile Send private message
christopher.wright
User


Joined: 17 Jun 2009
Posts: 927

PostPosted: Thu Jan 29, 2015 2:26 pm  Reply with quote

On Jan 29, 2015, at 5:21 AM, razmik.martirosyan wrote:

Quote:
Thanks Christopher, in other words are you also suggesting to
change the density unit?
There's no choice if you're to have consistent units.

Christopher Wright P.E. |"They couldn't hit an elephant at
chrisw@skypoint.com | this distance" (last words of Gen.
.......................................| John Sedgwick, Spotsylvania
1864)
http://www.skypoint.com/members/chrisw/



+-------------------------------------------------------------+
| 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
razmik.martirosyan
User


Joined: 17 Jun 2014
Posts: 43

PostPosted: Mon Feb 23, 2015 10:15 am  Reply with quote

Dear All,

During this time I was trying different simulations in order to solve my problem but all the
time I am facing a new one.

In case of CONTACT-TARGET:

I am defining contact surfaces under the concrete slab and imaginary subbase and the simulation goes well, but if the gravity is activated, there is a 'rigid body motion' error, and it shows that some node has a very big displacement, although the model seems to be contrained well.

In case of SPRINGS:

The only available spring element, LINK 180 is bringing the same rigid body motion error if it is used only in compression and I am not able to use it.

In case of SURF154:

Martin, I know you have suggested it first but I have tried to use it as a last option, my mistake probably. But I am not sure if I am using it in a right way. Should I select the below layer surface of my slab and by selecting nodes add SURF154 elements with EFS option? If Yes in this case how should I apply boundary conditions for those elements as they share same nodes with the slab?

Best Regards
Razmik Martirosyan
Universitat Polytechnica de Cataluña
Back to top
View user's profile Send private message
Martin Liddle
User


Joined: 15 Aug 2008
Posts: 1274
Location: Chesterfield, UK

PostPosted: Mon Feb 23, 2015 11:19 am  Reply with quote

On 23/02/2015 17:15, razmik.martirosyan wrote:
Quote:
I am defining contact surfaces under the concrete slab and imaginary subbase and the simulation goes well, but if the gravity is activated, there is a 'rigid body motion' error, and it shows that some node has a very big displacement, although the model seems to be contrained well.

So what units are you using now? Does the reaction force match your
hand calculation or is it orders of magnitude too big?


--
Martin Liddle, Tynemouth Computer Services,
Chesterfield, Derbyshire, UK.
www.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)
_________________
Martin Liddle, Tynemouth Computer Services,
Chesterfield, UK.
Back to top
View user's profile Send private message Visit poster's website
razmik.martirosyan
User


Joined: 17 Jun 2014
Posts: 43

PostPosted: Tue Feb 24, 2015 4:12 am  Reply with quote

Hi Martin,

I am using the ones I was using before i.e. MKS units, but with consideration.

I am doing static analysis, in each steo changing time by one unit as my properties are changing hourly, but I think I can make each step to be 3600(in seconds) so the time
will be in MKS also. Thus, I can use 9.8 for acel input (acel,0,9.8,0).

And as a result of rigid body motion error I am not getting converged solution to compare with something.

Best Regards
RAzmik Martirosyan
Universitat Polytechnica de Cataluña

Martin Liddle wrote:
On 23/02/2015 17:15, razmik.martirosyan wrote:
Quote:
I am defining contact surfaces under the concrete slab and imaginary subbase and the simulation goes well, but if the gravity is activated, there is a 'rigid body motion' error, and it shows that some node has a very big displacement, although the model seems to be contrained well.

So what units are you using now? Does the reaction force match your
hand calculation or is it orders of magnitude too big?


--
Martin Liddle, Tynemouth Computer Services,
Chesterfield, Derbyshire, UK.
www.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
jose.galan
User


Joined: 21 Oct 2008
Posts: 140

PostPosted: Tue Feb 24, 2015 8:21 am  Reply with quote

Dear Mr. Martirosyan,

you said that your simulation goes well, except when applying the
aceleration command. You do not mention the loading that you had on your
model when it worked well.

Have you tried replacing the vertical acceleration by an equivalent
uniform pressure?

You mentioned that you tried using link180 elements below the slab, and
you were also getting a rigid body motion error. I guess that you used
keyopt(2)=2 to obtaina a non-linear compression only behaviour. You
could try using keyopt(2)=0 (i.e. linear behaviour) to check if that
rigid body error is caused by the nonlinear behaviour of the spring, or
by an inadequately restrained model. Did you add one vertical link
element below each node on the slab? If so, your model lacks horizontal
and torsional restrains.

You may also check the values of stiffness that you are applying in your
nodes.

For link180, the axial stiffness (in N/m) is calculated as k=E*A/L,
where E is the young modulus (in Pa), defined as a material property, A
is the cross-sectional area of the link (in m^2), defined as real
constant and L is the element length (in m).

For your soil model, if you consider a constant modulus of subgrade
reaction KS (in N/m^3), the vertical stiffness under a node with an area
Anod (in m^2, obtained with the command ARNODE(N)) can be calculated as
k=KS*Anod.

Making both values equal, you can calculate the equivalent
cross-sectional area for the link180:

E*A/L=KS*Anod --> E*A=KS*Anod*L

A rough estimate of Ks measured on a plate test with a square plate of
30 cmx30 cm is between 10 and 100 MN/m^3. You could use KS=50
MN/m^3=50e9 N/m^3. Notice the large value of KS.

By the way, if you are solving a static analysis, the time does not have
any meaning, it is just an index to identify a load step. You may use
TIME,1 (in hours) or TIME,3600 (in seconds), it will not make any
difference. If you are solving a transient analysis, then time units
must be consistent.

If your time step is an hour, inertia is negligible and your structure
is responding statically. I would not perform a transient analysis.

In a static analysis, you must be careful to keep consistency of the
units, such taht mass*aceleration=density*volume*aceleration has units
of force. MKS is a safe bet.

Best regards,

Jose M. Galan

Assistant Prof.

Constr. Eng. Dept.

Univ. Sevilla

Spain


+-------------------------------------------------------------+
| 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
jose.galan
User


Joined: 21 Oct 2008
Posts: 140

PostPosted: Tue Feb 24, 2015 8:31 am  Reply with quote

There was a typo in my message: 50 MN=50e6 N

Jose M. Galan

Assistant Prof.

Constr. Eng. Dept.

Univ. Sevilla

Spain

El 24/02/2015 16:21, mfernan@us.es escribió:

Quote:
Dear Mr. Martirosyan,

you said that your simulation goes well, except when applying the
aceleration command. You do not mention the loading that you had on your
model when it worked well.

Have you tried replacing the vertical acceleration by an equivalent
uniform pressure?

You mentioned that you tried using link180 elements below the slab, and
you were also getting a rigid body motion error. I guess that you used
keyopt(2)=2 to obtaina a non-linear compression only behaviour. You
could try using keyopt(2)=0 (i.e. linear behaviour) to check if that
rigid body error is caused by the nonlinear behaviour of the spring, or
by an inadequately restrained model. Did you add one vertical link
element below each node on the slab? If so, your model lacks horizontal
and torsional restrains.

You may also check the values of stiffness that you are applying in your
nodes.

For link180, the axial stiffness (in N/m) is calculated as k=E*A/L,
where E is the young modulus (in Pa), defined as a material property, A
is the cross-sectional area of the link (in m^2), defined as real
constant and L is the element length (in m).

For your soil model, if you consider a constant modulus of subgrade
reaction KS (in N/m^3), the vertical stiffness under a node with an area
Anod (in m^2, obtained with the command ARNODE(N)) can be calculated as
k=KS*Anod.

Making both values equal, you can calculate the equivalent
cross-sectional area for the link180:

E*A/L=KS*Anod --> E*A=KS*Anod*L

A rough estimate of Ks measured on a plate test with a square plate of
30 cmx30 cm is between 10 and 100 MN/m^3. You could use KS=50
MN/m^3=50e6 N/m^3. Notice the large value of KS.

By the way, if you are solving a static analysis, the time does not have
any meaning, it is just an index to identify a load step. You may use
TIME,1 (in hours) or TIME,3600 (in seconds), it will not make any
difference. If you are solving a transient analysis, then time units
must be consistent.

If your time step is an hour, inertia is negligible and your structure
is responding statically. I would not perform a transient analysis.

In a static analysis, you must be careful to keep consistency of the
units, such taht mass*aceleration=density*volume*aceleration has units
of force. MKS is a safe bet.

Best regards,

Jose M. Galan

Assistant Prof.

Constr. Eng. Dept.

Univ. Sevilla

Spain

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