XANSYS Forum Index
    Register    

FAQ    Search    Memberlist    Usergroups    SmartFeedSmartFeed    Profile    Log in
[Xansys] EGEN command
 
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
irantzu.uriarte
User


Joined: 21 Oct 2008
Posts: 17

PostPosted: Mon Apr 06, 2009 3:35 am  Reply with quote

Dear all,

I'm trying to perform 3 meshes with the same element type (each one with its material properties) and the same nodes. I've used EGEN, saying 0 displacement; is it possible? Because it says that there's an error to plot elements.

Thanks in advance,
Irantzu

---------------------------
PhD. Student

EHU-UPV (Spain)

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


Joined: 21 Oct 2008
Posts: 17

PostPosted: Tue Apr 07, 2009 12:28 am  Reply with quote

Thank you for answering.

But I'm not sure if I understood the other post, I mean, I just want to
generate same element pattern, with same nodes. So I introduce:

EGEN,3,0,ALL,,,1 (1-> to introduce different material to each one)

Which is the error? (Doesn't this command duplicate elements?) Because I
can't see it.

Thank you once more,
Irantzu

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

PhD. Student

EHU-UPV (Spain)



-----Mensaje original-----
De: --email address suppressed-- [mailto:--email address suppressed--] En nombre
de Gururajarao, Raghavendran
Enviado el: lunes, 06 de abril de 2009 16:57
Para: ANSYS User Discussion List
Asunto: Re: [Xansys] EGEN command


>I'm trying to perform 3 meshes with the same element type (each one with
its
>material properties) and the same nodes. I've used EGEN, saying 0
>displacement; is it possible? Because it says that there's an error to plot
>elements.

Please have a look at one of the XANSYS discussion on the same lines at the
following link

http://www.xansys.org/forum/viewtopic.php?t=18737&highlight=egen

You may need to pay attention to the nodes generated. Hope this helps

Thanks
Raghavendran.G
Goodrich Aerospace India

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


Joined: 21 Oct 2008
Posts: 70

PostPosted: Tue Apr 07, 2009 1:20 am  Reply with quote

You could try this following command

mat,2 ! Set mat to 2 after the first set is generated

egen,3,,all,all,all,1,,,,,0,0,0 ! Material increment set to 1

After it has got generated you could issue

esel,s,mat,,2
esel,s,mat,,3 to check the elements

Please let me know if this works.

Thanks
Raghavendran.G
Goodrich Aerospace India

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


Joined: 21 Oct 2008
Posts: 17

PostPosted: Tue Apr 07, 2009 1:41 am  Reply with quote

I did it, but it doesn't work.

Well, with my try, if I do esel,s,p and go along the figure, the elements
are there, but I can't see them. So the problem maybe is just of graphics?

Thanks,
Irantzu

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

PhD. Student

EHU-UPV (Spain)


-----Mensaje original-----
De: --email address suppressed-- [mailto:--email address suppressed--] En nombre
de Gururajarao, Raghavendran
Enviado el: martes, 07 de abril de 2009 10:20
Para: ANSYS User Discussion List
Asunto: Re: [Xansys] EGEN command

You could try this following command



mat,2 ! Set mat to 2 after the first set is generated



egen,3,,all,all,all,1,,,,,0,0,0 ! Material increment set to 1



After it has got generated you could issue



esel,s,mat,,2

esel,s,mat,,3 to check the elements



Please let me know if this works.



Thanks

Raghavendran.G

Goodrich Aerospace India

+-------------------------------------------------------------+
| XANSYS web - www.xansys.org/forum |
| XANSYS blog - xansys.blogspot.com |
| The Online Community for users of ANSYS, Inc. Software |
| Hosted by PADT - www.padtinc.com |
| Send administrative requests to --email address suppressed-- |
+-------------------------------------------------------------+

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


Joined: 21 Oct 2008
Posts: 21

PostPosted: Tue Apr 07, 2009 4:45 am  Reply with quote

You need to generate nodes prior to elements.

Regards,

Roberto Porto
DSC Engenharia

----- Original Message -----
From: "Irantzu" <--email address suppressed-->
To: "'ANSYS User Discussion List'" <--email address suppressed-->
Sent: 07 April, 2009 4:28 AM
Subject: Re: [Xansys] EGEN command


> Thank you for answering.
>
> But I'm not sure if I understood the other post, I mean, I just want to
> generate same element pattern, with same nodes. So I introduce:
>
> EGEN,3,0,ALL,,,1 (1-> to introduce different material to each one)
>
> Which is the error? (Doesn't this command duplicate elements?) Because I
> can't see it.
>
> Thank you once more,
> Irantzu
>
> ---------------------------
>
> PhD. Student
>
> EHU-UPV (Spain)
>
>
>
> -----Mensaje original-----
> De: --email address suppressed-- [mailto:--email address suppressed--] En nombre
> de Gururajarao, Raghavendran
> Enviado el: lunes, 06 de abril de 2009 16:57
> Para: ANSYS User Discussion List
> Asunto: Re: [Xansys] EGEN command
>
>
>>I'm trying to perform 3 meshes with the same element type (each one with
> its
>>material properties) and the same nodes. I've used EGEN, saying 0
>>displacement; is it possible? Because it says that there's an error to
>>plot
>>elements.
>
> Please have a look at one of the XANSYS discussion on the same lines at
> the
> following link
>
> http://www.xansys.org/forum/viewtopic.php?t=18737&highlight=egen
>
> You may need to pay attention to the nodes generated. Hope this helps
>
> Thanks
> Raghavendran.G
> Goodrich Aerospace India
>
>
>
> +-------------------------------------------------------------+
> | XANSYS web - www.xansys.org/forum |
> | XANSYS blog - xansys.blogspot.com |
> | The Online Community for users of ANSYS, Inc. Software |
> | Hosted by PADT - www.padtinc.com |
> | Send administrative requests to --email address suppressed-- |
> +-------------------------------------------------------------+
>
>

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





PostPosted: Tue Apr 07, 2009 7:18 am  Reply with quote

On Apr 7, 2009, at 2:28 AM, Irantzu wrote:

> But I'm not sure if I understood the other post, I mean, I just
> want to
> generate same element pattern, with same nodes. So I introduce:
>
> EGEN,3,0,ALL,,,1 (1-> to introduce different material to each one)
>
> Which is the error? (Doesn't this command duplicate elements?)
> Because I
> can't see it.
Sounds like you've generated elements but not nodes. Could be you've
made the new set coincident with the old set with the node increment
defaulting to zero. Or maybe ANSYS realized that you'd screwed up and
did nothing.I'm assuming you're using Classic and not the Black Box.

Sensible practice in cases where something unexpected happens is to
look at the output listing (not the log file) to see how ANSYS has
reacted to the command. If you're looking at the screen the program's
response to your command may flash by too quickly or the display may
be too abbreviated. It's an old trick, but it just might work.

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

Post generated using Mail2Forum (http://www.mail2forum.com)
Back to top
irantzu.uriarte
User


Joined: 21 Oct 2008
Posts: 17

PostPosted: Tue Apr 07, 2009 7:42 am  Reply with quote

Hello again, and thanks for answering (being mine maybe a fool question...).

I did first VMESH, so the nodes exist.

Then, I introduce EGEN, and 0 in first node's place, to overwrite
them, because I just want those nodes to appear once.

The response of the program is that the eplot command can not be
displayed or something similar (because powergraphics doesn't support
that command...). So if I write ESEL,S,P and I locate the mouse on the
solid, it says that there exist 3 elements in one of them for example.
So it seems that the elements are created, but not plotted. Why occurs
this??

Sorry if it's a stupid question, but I'm a little bit lost...



Christopher Wright <--email address suppressed--> ha escrito:

>
> On Apr 7, 2009, at 2:28 AM, Irantzu wrote:
>
>> But I'm not sure if I understood the other post, I mean, I just
>> want to
>> generate same element pattern, with same nodes. So I introduce:
>>
>> EGEN,3,0,ALL,,,1 (1-> to introduce different material to each one)
>>
>> Which is the error? (Doesn't this command duplicate elements?)
>> Because I
>> can't see it.
> Sounds like you've generated elements but not nodes. Could be you've
> made the new set coincident with the old set with the node increment
> defaulting to zero. Or maybe ANSYS realized that you'd screwed up and
> did nothing.I'm assuming you're using Classic and not the Black Box.
>
> Sensible practice in cases where something unexpected happens is to
> look at the output listing (not the log file) to see how ANSYS has
> reacted to the command. If you're looking at the screen the program's
> response to your command may flash by too quickly or the display may
> be too abbreviated. It's an old trick, but it just might work.
>
> Christopher Wright P.E. |"They couldn't hit an elephant at
> --email address suppressed-- | this distance" (last words of Gen.
> .......................................| John Sedgwick, Spotsylvania
> 1864)
> http://www.skypoint.com/members/chrisw/
>
>
> +-------------------------------------------------------------+
> | XANSYS web - www.xansys.org/forum |
> | XANSYS blog - xansys.blogspot.com |
> | The Online Community for users of ANSYS, Inc. Software |
> | Hosted by PADT - www.padtinc.com |
> | Send administrative requests to --email address suppressed-- |
> +-------------------------------------------------------------+
>
>

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


Joined: 05 Feb 2009
Posts: 100

PostPosted: Tue Apr 07, 2009 7:53 am  Reply with quote

Identical overlapping elements confuse the Ansys plotting routine. To make the elements appear type in, "/SHRINK,.001"
Keith
Keith DiRienz
Office: 949.481.4946
FEA Technologies
http://members.cox.net/fea-technologies

At 07:42 AM 4/7/2009, you wrote:
Hello again, and thanks for answering (being mine maybe a fool question...).

I did first VMESH, so the nodes exist.

Then, I introduce EGEN, and 0 in first node's place, to overwrite
them, because I just want those nodes to appear once.

The response of the program is that the eplot command can not be
displayed or something similar (because powergraphics doesn't support
that command...). So if I write ESEL,S,P and I locate the mouse on the
solid, it says that there exist 3 elements in one of them for example.
So it seems that the elements are created, but not plotted. Why occurs
this??

Sorry if it's a stupid question, but I'm a little bit lost...
(end of quote)

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





PostPosted: Tue Apr 07, 2009 7:54 am  Reply with quote

On Apr 7, 2009, at 9:42 AM, Irantzu Uriarte Gallastegui wrote:

>
> I did first VMESH, so the nodes exist.
Just look at the output listing to see what happened.


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

Post generated using Mail2Forum (http://www.mail2forum.com)
Back to top
raghavendran.g
User


Joined: 21 Oct 2008
Posts: 70

PostPosted: Tue Apr 07, 2009 8:24 am  Reply with quote

In your case as you needed overlapping elements with same set of nodes you had used EGEN command. If you need to display the elements that you have created, try the following

Option-1

/device,vector,on (! This will display all the elements in Wireframe mode)

Option-2

esel,r,mat,,1
allsel,belo,elem
eplot !(this should display the elements with powergraphics on or off mode too)

Could you please let the list know something more about the objective of the analysis (If it is not confidential), I believe you may get other good approaches

Best of Luck

Thanks
Raghavendran.G
Goodrich Aerospace India

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 Apr 07, 2009 8:25 am  Reply with quote

Dear Irantzu,
when using the egen command, Ansys delivers a warning message "Overlapping elements will be generated due to zero node increment".
You can check with the command ELIST that the new elements are in fact in your model. You can distinguish them by looking at the second column, that corresponds to its material. However, Ansys issues a warning message when you try to plot them if they are all selected. The only way to plot them is by selecting only one material at a time. In that manner, you avoid overlapping elements in the selected set.
For example, if you want to see the elements with material 2:

/PNUM,ELEM,1     !Show element numbers

ESEL,S,MAT,,2

EPLOT


If you want to see elements with material 3:

ESEL,S,MAT,,3

EPLOT

You will notice the change in element numbers after the latter eplot command.



Please, check the following section of the Ansys manual

Modeling and Meshing Guide | Chapter 9. Direct Generation |  9.2. Elements


It contains some comments about the problems that you may encounter when using overlapping elements. The following paragraph is copied directly from the manual.

9.2.4. A Note About Overlapping Elements
Be advised that if you create overlapping elements (that is, elements attached to the same nodes and occupying the same space), various ANSYS features such as graphics, surface loads, selecting logic, etc. might not function as expected. It is best to avoid the use of overlapping elements altogether; if this is not possible, use extreme caution whenever you employ overlapping elements.


Best regards,

Jose M. Galan
Department of Construction Engineering 
Escuela Tecnica Superior de Ingenieros 
University of Sevilla 
Spain 

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


Joined: 21 Oct 2008
Posts: 17

PostPosted: Wed Apr 08, 2009 12:05 am  Reply with quote

Dear all,

Thanks a lot. Finally, when I introduced what Keith said, I could "see" the
elements. (I had tried to do what Jose M. has proposed (previously) but it
didn't work.)

Raghavendran, I'm trying to model (carbon-black) filled rubber, taking into
account hyperelasticity, viscoelasticity and plasticity (one mesh for each
of the behaviours).

Best regards,
Irantzu

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

PhD. Student

EHU-UPV (Spain)


-----Mensaje original-----
De: --email address suppressed-- [mailto:--email address suppressed--] En nombre
de Jose M. Galan
Enviado el: martes, 07 de abril de 2009 17:37
Para: ANSYS User Discussion List
Asunto: Re: [Xansys] EGEN command

Dear Irantzu,
when using the egen command, Ansys delivers a warning message "Overlapping
elements will be generated due to zero node increment".
You can check with the command ELIST that the new elements are in fact in
your
model. You can distinguish them by looking at the second column, that
corresponds to
its material. However, Ansys issues a warning message when you try to plot
them if
they are all selected. The only way to plot them is by selecting only one
material at a
time. In that manner, you avoid overlapping elements in the selected set.
For example, if you want to see the elements with material 2:

/PNUM,ELEM,1 !Show element numbers

ESEL,S,MAT,,2

EPLOT


If you want to see elements with material 3:

ESEL,S,MAT,,3

EPLOT

You will notice the change in element numbers after the latter eplot
command.



Please, check the following section of the Ansys manual

Modeling and Meshing Guide | Chapter 9. Direct Generation | 9.2. Elements


It contains some comments about the problems that you may encounter when
using
overlapping elements. The following paragraph is copied directly from the
manual.

9.2.4. A Note About Overlapping Elements
Be advised that if you create overlapping elements (that is, elements
attached to the
same nodes and occupying the same space), various ANSYS features such as
graphics, surface loads, selecting logic, etc. might not function as
expected. It is best to
avoid the use of overlapping elements altogether; if this is not possible,
use extreme
caution whenever you employ overlapping elements.


Best regards,

Jose M. Galan
Department of Construction Engineering
Escuela Tecnica Superior de Ingenieros
University of Sevilla
Spain

+-------------------------------------------------------------+
| XANSYS web - www.xansys.org/forum |
| XANSYS blog - xansys.blogspot.com |
| The Online Community for users of ANSYS, Inc. Software |
| Hosted by PADT - www.padtinc.com |
| Send administrative requests to --email address suppressed-- |
+-------------------------------------------------------------+

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