XANSYS Forum Index
    Register    

FAQ    Search    Memberlist    Usergroups    SmartFeedSmartFeed    Profile    Log in
Assigning SOLID65 to triangular mesh
 
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
yannis.gkiokas
User


Joined: 17 Jun 2014
Posts: 22

PostPosted: Thu Jul 03, 2014 1:21 am  Reply with quote

Dear All,

Hallo. I have the geometry of an arch defined with 500 nodes and the mesh which is made with triangular elements. These i cannot change.

The Problem is that i want to assign a Drucker Prager model on that arch, which goes only with SOLID65 elements. Of course as you know, these elements are Quads and require 4 nodes to be defined in an element. As said i cannot change the definition of the elements i was given, they must remain triangulars. How could i apply thus Drucker Prager to my geometry?

Any proposals?


Best Regards,
_________________
Yannis Gkiokas
Dipl. Ing Technical University Munich
Master Student
Back to top
View user's profile Send private message Send e-mail
jose.galan
User


Joined: 21 Oct 2008
Posts: 140

PostPosted: Thu Jul 03, 2014 4:08 am  Reply with quote

Dear Mr. Gkiokas,
in previous versions of Ansys the Drucker-Prager model (TB,DP) could also be applied to some PLANE elements.

In Ansys 11 help, it mentions the following:
"DP — Drucker-Prager plasticity (LINK1, LINK8, PIPE20, BEAM23, BEAM24, PLANE42, SHELL43, SOLID45, PIPE60, SOLID62, SOLID65, PLANE82, SHELL91, SOLID92, SHELL93, SOLID95, and PLANE183). See "DP Specifications" for more information"

On the other hand, in the Ansys 15 manual, for DP plasticity it only shows SOLID65, as you have already found out. (Mechanical APDL> Material Reference > 2. Material Model Element support.)

However, EDP can be used with several plane elements (PLANE182, 183, 223). You could use EDP with linear yield and flow criteria, and define adequately the material constants to be equivalent to a DP material. You can obtain the relationship between the material constants by comparing the definitions of F and Q in both models.
You can find them in Mechanical APDL>Theory reference > 4. Structures with nonlinearities > 4.2.16 Specialization for Drucker-Prager
EDP does not include the dilatancy angle that is available in DP. In EDP with linear F and Q forms, it is assumed to be equal to the friction angle.

I guess that you could still use the DP model as in ansys 11 version (even when undocumented in v15), but you should check it first.

Best regards,
Jose M. Galan
Constr. Eng. Dept.
Univ. Sevilla
Spain
Back to top
View user's profile Send private message
yannis.gkiokas
User


Joined: 17 Jun 2014
Posts: 22

PostPosted: Thu Jul 03, 2014 5:25 am  Reply with quote

Dear Mr Galan,

I am using ANSYS 14.5. In Ansys help i have found out that PIPE289 is defined from 3 nodes and can be used with EDP and MISO or BISO.

But i have a Problem in defining it. I get the error :
#Line Element1 has a Zero or negative determinant of the Jacobian Matrix at one of ist sampling Locations. The midside node may be poorly positioned.#

As said, i have all the 500 nodes in x,y,z coordinates and this element type suits.

Would you help on defining PIPE289?

*About DP , i have checked the elements you say and only SOLID65 supports it in ANSYS14.5

Regards,
_________________
Yannis Gkiokas
Dipl. Ing Technical University Munich
Master Student
Back to top
View user's profile Send private message Send e-mail
jose.galan
User


Joined: 21 Oct 2008
Posts: 140

PostPosted: Thu Jul 03, 2014 6:13 am  Reply with quote

Dear Mr. Gkiokas,
in your first post you said that you had a mesh of triangular elements of an arch. That means that you have a plane model. You should use PLANE elements. PIPE289 is a line element, similar to a beam element. Therefore, it is not applicable to triangular elements, only to line elements. Please, have a look at the ansys help on pipe289 and compare it with PLANE182.


You can also try to use the old Ansys elements, even when they do not longer appear in the manual. Try this:
et,1,plane42 !2d 3- or 4-node plane stress element
!It is an old version of plane182
tb,dp,1
tbdata,,cohesion,angleinternalfrict,dilatancyangle


Best regards,

Jose M. Galan

Constr. Eng. Dept.

Univ. Sevilla

Spain
Back to top
View user's profile Send private message
yannis.gkiokas
User


Joined: 17 Jun 2014
Posts: 22

PostPosted: Thu Jul 03, 2014 7:21 am  Reply with quote

Dear Mr Galan,

yes i was given the nodes i.e. n,1,23,34,32 , n,2,25,37,46, etc

and the elements (they are defined by three nodes) i.e e,1,3,7 , e,2,5,9 etc...

The thing is i want to apply a plasticity material model in my arch(EDP or DP);
but i have to be careful because i have to pay attention to two restrictions:
1) I have to apply a material model that supports triangular mesh , and

2)Not easily the plasticity models go along with 3-node elements.

P.s About PLANE182 it is said that it goes with EDP, but only for plane stress.Is it ok for me?

Best Regards,
_________________
Yannis Gkiokas
Dipl. Ing Technical University Munich
Master Student
Back to top
View user's profile Send private message Send e-mail
jose.galan
User


Joined: 21 Oct 2008
Posts: 140

PostPosted: Thu Jul 03, 2014 10:18 am  Reply with quote

Dear Mr. Gkiokas,

in the ansys manual says that EDP in PLANE182 (and PLANE183) is not
applicable for plane stress, just the opposite of what you said in your
post. PLANE182 provides other element behaviours (plane strain,
generalized plane strain, axisymmetric) that are selected by providing
an appropiate value to the KEYOPT(3). Please, see ansys manual
information on that element.

If you have a mesh of 3-node triangles, PLANE182 is your element.

Make sure that the behaviour that you choose represents the actual
conditions of your structure.

Best regards,

Jose M. Galan

Constr. Eng. Dept.

Univ. Sevilla

Spain

El 03/07/2014 16:21, yannis.gkiokas escribió:

Quote:
Dear Mr Galan,

yes i was given the nodes i.e. n,1,23,34,32 , n,2,25,37,46, etc

and the elements (they are defined by three nodes) i.e e,1,3,7 , e,2,5,9 etc...

The thing is i want to apply a plasticity material model in my arch(EDP or DP);
but i have to be careful because i have to pay attention to two restrictions:
1) I have to apply a material model that supports triangular mesh , and

2)Not easily the plasticity models go along with 3-node elements.

P.s About PLANE182 it is said that it goes with EDP, but only for plane stress.Is it ok for me?

Best Regards,

------------------------
Yannis Gkiokas
Dipl. Ing Technical University Munich
Master Student

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