Hello everyone,
I hope you can solve my problem. I need to calculate the volume change of a box subjected to pressure on all its internal faces. I have simply created a parallelepiped and modeled it with shell elements. I applied the pressure to all the internal faces of the box and solved it.
Is there a way to calculate the volume change of the box?
Thank you for you help and time.
Best regards,
Francesca
Student at Politecnico di Torino

Unless I am very wrong, I don’t think that there is a direct way to do it.

One possible way is to extract the locations of your nodes before and after
the loading is applied. Then you might need some surface numerical
integration to get the volume. Remember, the volume is the integral of a
varying area over length.

I hope this helps.

Best,
Mohammad

---====
Mohammad A Gharaibeh, Ph.D.
Associate Professor
Department of Mechanical Engineering
The Hashemite University
P.O. Box 330127
Zarqa, 13133, Jordan
Tel: +962 - 5 - 390 3333 Ext. 4771
Fax: +962 - 5 - 382 6348

---====

Hi Francesca.

You could try something like this (rough idea):

• Model and mesh the box and a surrounding volume, meaning you have a volume with the box embedded (I think both box and surrounding volume should be solid elements, and they should definitely be sharing nodes).
• The surrounding solid elements should have approx. zero stiffness, so they do not resist the deformation of the box.
• Apply the internal pressure, run the analysis.
• In a copy of the meshed model, use UPGEOM to update the nodes according to the deformed model from the first analysis.
• Measure the volume of only the surrounding solid elements with updated node positions.

If you had to do it with a shell element box (still solid element surrounding), you would need to compensate for a half thickness due to the mid-surface shell.

The accuracy of all this would depend on the deformation of the box. If it is excessive compared to the surrounding solid elements, you may have some problems with convergence, collapsing solid elements etc.

Good luck.

Uffe Dal Eriksen
Ramboll Energy Transition,
Denmark

Classification: Confidential
-----Original Message-----
From: Francesca Pistorio via Xansys xansys-temp@list.xansys.org
Sent: 4. juli 2024 18:09
To: xansys-temp@list.xansys.org
Cc: Francesca Pistorio francesca.pistorio@polito.it
Subject: [Xansys] Volume variation computation

Hello everyone,
I hope you can solve my problem. I need to calculate the volume change of a box subjected to pressure on all its internal faces. I have simply created a parallelepiped and modeled it with shell elements. I applied the pressure to all the internal faces of the box and solved it.
Is there a way to calculate the volume change of the box?
Thank you for you help and time.
Best regards,
Francesca
Student at Politecnico di Torino

Xansys mailing list -- xansys-temp@list.xansys.org To unsubscribe send an email to xansys-temp-leave@list.xansys.org If you are receiving too many emails from XANSYS please consider changing account settings to Digest mode which will send a single email per day.

Please send administrative requests such as deletion from XANSYS to xansys-mod@tynecomp.co.uk and not to the list

I'm fairly sure newer versions of Workbench allow you to export deformed shape geometry.  And you can export it to a new system to run a new analysis.  In that case, the downstream system should report the volume of the deformed structures in the Geometry branch properties.  But in your case with an open box, I think you would have to create an "soft" body (i.e., low modulus) inside the open box that follows the shape of the deformation.  And you would have to dither on its volume in the downstream system.

-Matt

-----Original Message-----
From: Francesca Pistorio via Xansys xansys-temp@list.xansys.org
Sent: Thursday, July 4, 2024 12:09 PM
To: xansys-temp@list.xansys.org
Cc: Francesca Pistorio francesca.pistorio@polito.it
Subject: [Xansys] Volume variation computation

Hello everyone,
I hope you can solve my problem. I need to calculate the volume change of a box subjected to pressure on all its internal faces. I have simply created a parallelepiped and modeled it with shell elements. I applied the pressure to all the internal faces of the box and solved it.
Is there a way to calculate the volume change of the box?
Thank you for you help and time.
Best regards,
Francesca
Student at Politecnico di Torino

Xansys mailing list -- xansys-temp@list.xansys.org To unsubscribe send an email to xansys-temp-leave@list.xansys.org If you are receiving too many emails from XANSYS please consider changing account settings to Digest mode which will send a single email per day.

Please send administrative requests such as deletion from XANSYS to xansys-mod@tynecomp.co.uk and not to the list

Hi Francesca, Hi Uffe,

I was about to suggest Uffe's way, except I would mesh internal volume instead of surrounding. This way the volume you are looking for is directly that of the deformed "air" volume, that you can get with  ETABLE,volume,VOLU  $  SSUM  after a solve on deformed mesh using 0 pressure.

Best regards,

David Galindo
PHAREA ceo

-----Message d'origine-----
De : Uffe Dal Eriksen via Xansys xansys-temp@list.xansys.org
Envoyé : vendredi 5 juillet 2024 08:32
À : XANSYS Mailing List Home xansys-temp@list.xansys.org
Cc : Uffe Dal Eriksen UDE@ramboll.com
Objet : [Xansys] Re: Volume variation computation

Hi Francesca.

You could try something like this (rough idea):

• Model and mesh the box and a surrounding volume, meaning you have a volume with the box embedded (I think both box and surrounding volume should be solid elements, and they should definitely be sharing nodes).
• The surrounding solid elements should have approx. zero stiffness, so they do not resist the deformation of the box.
• Apply the internal pressure, run the analysis.
• In a copy of the meshed model, use UPGEOM to update the nodes according to the deformed model from the first analysis.
• Measure the volume of only the surrounding solid elements with updated node positions.

If you had to do it with a shell element box (still solid element surrounding), you would need to compensate for a half thickness due to the mid-surface shell.

The accuracy of all this would depend on the deformation of the box. If it is excessive compared to the surrounding solid elements, you may have some problems with convergence, collapsing solid elements etc.

Good luck.

Uffe Dal Eriksen
Ramboll Energy Transition,
Denmark

Classification: Confidential
-----Original Message-----
From: Francesca Pistorio via Xansys xansys-temp@list.xansys.org
Sent: 4. juli 2024 18:09
To: xansys-temp@list.xansys.org
Cc: Francesca Pistorio francesca.pistorio@polito.it
Subject: [Xansys] Volume variation computation

Hello everyone,
I hope you can solve my problem. I need to calculate the volume change of a box subjected to pressure on all its internal faces. I have simply created a parallelepiped and modeled it with shell elements. I applied the pressure to all the internal faces of the box and solved it.
Is there a way to calculate the volume change of the box?
Thank you for you help and time.
Best regards,
Francesca
Student at Politecnico di Torino

Xansys mailing list -- xansys-temp@list.xansys.org To unsubscribe send an email to xansys-temp-leave@list.xansys.org If you are receiving too many emails from XANSYS please consider changing account settings to Digest mode which will send a single email per day.

Please send administrative requests such as deletion from XANSYS to xansys-mod@tynecomp.co.uk and not to the list _______________________________________________
Xansys mailing list -- xansys-temp@list.xansys.org To unsubscribe send an email to xansys-temp-leave@list.xansys.org If you are receiving too many emails from XANSYS please consider changing account settings to Digest mode which will send a single email per day.

Please send administrative requests such as deletion from XANSYS to xansys-mod@tynecomp.co.uk and not to the list

Hi all,

And if you are using ANSYS Workbench, there is a custom user defined result for VOLU.
If associated with solid elements, it represents each elements volume.
If associated with shell elements, it represents each elements area.

Regards,
Irene Slater
Corning Incorporated

-----Original Message-----
From: David GALINDO - Pharea via Xansys xansys-temp@list.xansys.org
Sent: Friday, July 5, 2024 4:48 AM
To: XANSYS Mailing List Home xansys-temp@list.xansys.org
Cc: Uffe Dal Eriksen UDE@ramboll.com; David GALINDO - Pharea d.galindo@pharea.com
Subject: [⚠️] [EXTERNAL]--[Xansys] Re: Volume variation computation

Caution: This email originated from outside of Corning. Do not click links or open attachments unless you recognize the sender and know the content is safe. Report phishing by using the “Report Phishing” button or forward the email to Phishyemails@corning.com.

Hi Francesca, Hi Uffe,

I was about to suggest Uffe's way, except I would mesh internal volume instead of surrounding. This way the volume you are looking for is directly that of the deformed "air" volume, that you can get with  ETABLE,volume,VOLU  $  SSUM  after a solve on deformed mesh using 0 pressure.

Best regards,

David Galindo
PHAREA ceo

-----Message d'origine-----
De : Uffe Dal Eriksen via Xansys xansys-temp@list.xansys.org Envoyé : vendredi 5 juillet 2024 08:32 À : XANSYS Mailing List Home xansys-temp@list.xansys.org Cc : Uffe Dal Eriksen UDE@ramboll.com Objet : [Xansys] Re: Volume variation computation

Hi Francesca.

You could try something like this (rough idea):

• Model and mesh the box and a surrounding volume, meaning you have a volume with the box embedded (I think both box and surrounding volume should be solid elements, and they should definitely be sharing nodes).
• The surrounding solid elements should have approx. zero stiffness, so they do not resist the deformation of the box.
• Apply the internal pressure, run the analysis.
• In a copy of the meshed model, use UPGEOM to update the nodes according to the deformed model from the first analysis.
• Measure the volume of only the surrounding solid elements with updated node positions.

If you had to do it with a shell element box (still solid element surrounding), you would need to compensate for a half thickness due to the mid-surface shell.

The accuracy of all this would depend on the deformation of the box. If it is excessive compared to the surrounding solid elements, you may have some problems with convergence, collapsing solid elements etc.

Good luck.

Uffe Dal Eriksen
Ramboll Energy Transition,
Denmark

Classification: Confidential
-----Original Message-----
From: Francesca Pistorio via Xansys xansys-temp@list.xansys.org
Sent: 4. juli 2024 18:09
To: xansys-temp@list.xansys.org
Cc: Francesca Pistorio francesca.pistorio@polito.it
Subject: [Xansys] Volume variation computation

Hello everyone,
I hope you can solve my problem. I need to calculate the volume change of a box subjected to pressure on all its internal faces. I have simply created a parallelepiped and modeled it with shell elements. I applied the pressure to all the internal faces of the box and solved it.
Is there a way to calculate the volume change of the box?
Thank you for you help and time.
Best regards,
Francesca
Student at Politecnico di Torino

Xansys mailing list -- xansys-temp@list.xansys.org To unsubscribe send an email to xansys-temp-leave@list.xansys.org If you are receiving too many emails from XANSYS please consider changing account settings to Digest mode which will send a single email per day.

Please send administrative requests such as deletion from XANSYS to xansys-mod@tynecomp.co.uk and not to the list _______________________________________________
Xansys mailing list -- xansys-temp@list.xansys.org To unsubscribe send an email to xansys-temp-leave@list.xansys.org If you are receiving too many emails from XANSYS please consider changing account settings to Digest mode which will send a single email per day.

Please send administrative requests such as deletion from XANSYS to xansys-mod@tynecomp.co.uk and not to the list _______________________________________________
Xansys mailing list -- xansys-temp@list.xansys.org To unsubscribe send an email to xansys-temp-leave@list.xansys.org If you are receiving too many emails from XANSYS please consider changing account settings to Digest mode which will send a single email per day.

Please send administrative requests such as deletion from XANSYS to xansys-mod@tynecomp.co.uk and not to the list

Well, a simple question to the ChatGPT provided a reasonable solution
(below). Please note that I didn't check the sanity of this.

To calculate the volume change of a box subjected to internal pressure
using ANSYS with shell elements, you can follow these steps:

Method 1: Using Displacement Data

1. Post-Processing Displacement Data:

   • Once you have solved the model, obtain the nodal displacement data
     from the solution. This can be done in the ANSYS post-processor (ANSYS
     Mechanical or ANSYS APDL).

2. Calculate New Node Positions:

   • Use the displacement data to calculate the new positions of the nodes
     after deformation.

3. Reconstruct the Deformed Shape:

   • Using the new node positions, reconstruct the deformed geometry of the
     box. For shell elements, you'll need to account for the mid-surface
     displacements.

4. Calculate the Deformed Volume:

   • If your initial box dimensions are known, you can compute the initial
     volume (V_0). For a box with length (L), width (W), and height (H),
     the volume is:
     [
     V_0 = L \times W \times H
     ]
   • To find the deformed volume (V_d), you can create a solid
     representation of the deformed shell structure and use a volume calculation
     tool within ANSYS or export the deformed geometry to a CAD tool that can
     calculate the volume of complex shapes.

Method 2: Using Strain Data

1. Obtain Strain Data:

   • Extract the volumetric strain data from the solution. Volumetric
     strain ((\epsilon_v)) can be obtained from the strain components (usually
     in the strain tensor output). It is the trace of the strain tensor:
     [
     \epsilon_v = \epsilon_x + \epsilon_y + \epsilon_z
     ]

2. Calculate Volume Change:

   • The change in volume (\Delta V) can be related to the initial volume
     (V_0) and the volumetric strain (\epsilon_v) as follows:
     [
     \Delta V = V_0 \times \epsilon_v
     ]
   • The deformed volume (V_d) is then:
     [
     V_d = V_0 + \Delta V = V_0 (1 + \epsilon_v)
     ]

Step-by-Step Procedure in ANSYS:

1. Solve the Model:

   • Apply the pressure on the internal faces of the box and solve the
     finite element model.

2. Post-Processing:

   • Go to the post-processor in ANSYS.

3. Extract Displacement Data:

   • Export the nodal displacement data.
   • Calculate the new node positions and reconstruct the deformed shape.
   • OR

4. Extract Strain Data:

   • Get the volumetric strain data for the elements.

5. Volume Calculation:

   • If using displacement data, use a CAD tool or ANSYS to find the
     deformed volume.
   • If using strain data, compute the deformed volume using the volumetric
     strain as described.

ANSYS APDL Example Code:

If you are using ANSYS APDL, you can use the following steps:

1. Apply Pressure and Solve:

   /prep7
   ! Define geometry, materials, and apply pressure
   et,1,shell281
   keyopt,1,8,1  ! Use full integration points
   ! Define geometry, meshing, boundary conditions, and loads
   ...
   /solu
   solve
   finish
   

2. Post-Processing for Displacement:

   /post1
   set,last
   *get,nnode,node,,count  ! Number of nodes
   *dim,disp,array,nnode,3  ! Create array to store displacements
   *vget,disp(1,1),node,1,ux
   *vget,disp(1,2),node,1,uy
   *vget,disp(1,3),node,1,uz
   *dim,newpos,array,nnode,3  ! Array for new positions
   *do,i,1,nnode
      *get,xpos,node,i,loc,x
      *get,ypos,node,i,loc,y
      *get,zpos,node,i,loc,z
      newpos(i,1) = xpos + disp(i,1)
      newpos(i,2) = ypos + disp(i,2)
      newpos(i,3) = zpos + disp(i,3)
   *enddo
   ! Export new positions for volume calculation
   

3. Post-Processing for Strain:

   /post1
   set,last
   *get,nelem,elem,,count  ! Number of elements
   *dim,volstrain,array,nelem  ! Array to store volumetric strain
   *vget,volstrain(1),elem,1,eptemp ! Assuming vol strain is stored in
   

eptemp
*dim,elemvol,array,nelem  ! Array to store element volumes
*vget,elemvol(1),elem,1,volu
*dim,totalvolstrain,array,1  ! Total volumetric strain
*voper,totalvolstrain(1),volstrain,elemvol,sum
*get,totvolsum,elem,0,volu,sum
totalvol = totalvolstrain/totvolsum  ! Average volumetric strain
*stat,totalvol

4. **Calculate Deformed Volume**:
```apdl
V0 = initial_volume  ! Define the initial volume of the box
Vd = V0 * (1 + totalvol)  ! Deformed volume
*stat,Vd

By following these steps, you can calculate the volume change of the box
subjected to internal pressure using ANSYS. If you have specific initial
dimensions or additional details about the setup, those can be incorporated
into the calculations accordingly.

--

Mohammad

---====
Mohammad A Gharaibeh, Ph.D.
Associate Professor
Department of Mechanical Engineering
The Hashemite University
P.O. Box 330127
Zarqa, 13133, Jordan
Tel: +962 - 5 - 390 3333 Ext. 4771
Fax: +962 - 5 - 382 6348

---====

Hi,

In order to explicit the method I propose, here is the script for a 1x1x1 box meshed with shell181 and its internal volume with solid185.
Shell thickness is not considered in volume calculation since this is not an issue.
Last command returns the deformed volume in the output window.
Note that at the end of this script the undeformed model is lost. Files could be copied after 1st solve to keep model and results.

!*** modelling box and solving under internal pressure, not the interesting part so I use some $ for less lines
!*** Just note the model is a shell box which internal volume is meshed with near 0 stiffness 3D elements

fini $ /clear $ /prep7
block,0,1,0,1,0,1 $ esize,0.1
et,1,181 $ sectype,1,shell,,box $ secdata,0.01 $ mp,ex,1,200e9 $ mp,prxy,1,0.3
et,2,185 $ mp,ex,2,1 $ mp,prxy,2,0.3
type,1 $ secnum,1 $ mat,1 $ amesh,all
type,2 $ secnum,2 $ mat,2 $ vmesh,all
esel,s,ename,,181 $ sfe,all,1,pres,0,1e5 $ d,node(0,0,0),all,all,0
fini $ /solu $ allsel $ solve

!*****************************************************
!*** Start of the interesting part *******************
!*****************************************************

fini
/prep7

allsel

upgeom,1,last,last,file,rst    ! update mesh to match the deformed shape obtained from applied pressure

fini
/solu

esel,s,ename,,181
sfe,all,1,pres,0,0              ! run a 2nd solve with 0 pressure
allsel
solve

fini
/post1

esel,s,ename,,185
etable,volume,volu              ! sort volume of 3D elements
ssum

Best regards,
David Galindo
PHAREA ceo

De : Dr. Juan Pablo Toledo Gonzalez juan.toledo@complx.com.mx
Envoyé : vendredi 5 juillet 2024 22:42
À : XANSYS Mailing List Home xansys-temp@list.xansys.org
Cc : Uffe Dal Eriksen UDE@ramboll.com; David GALINDO - Pharea d.galindo@pharea.com
Objet : Re: [Xansys] Re: Volume variation computation

Hi Francesca ,

You could add a Commands (APDL) option and then use the *get command, to obtain node displancement hence calculate the new volume.

Regards,

General Manager
COMPLX
"Ingeniería Avanzada para Soluciones Reales"
www.complx.com.mxhttp://www.complx.com.mx/
Tel: 229 337 1365
Cel: 229 136 5599

El 2024-07-05 02:47, David GALINDO - Pharea via Xansys escribió:
Hi Francesca, Hi Uffe,

I was about to suggest Uffe's way, except I would mesh internal volume instead of surrounding. This way the volume you are looking for is directly that of the deformed "air" volume, that you can get with  ETABLE,volume,VOLU  $  SSUM  after a solve on deformed mesh using 0 pressure.

Best regards,

David Galindo
PHAREA ceo

-----Message d'origine-----
De : Uffe Dal Eriksen via Xansys <xansys-temp@list.xansys.orgmailto:xansys-temp@list.xansys.org>
Envoyé : vendredi 5 juillet 2024 08:32
À : XANSYS Mailing List Home <xansys-temp@list.xansys.orgmailto:xansys-temp@list.xansys.org>
Cc : Uffe Dal Eriksen <UDE@ramboll.commailto:UDE@ramboll.com>
Objet : [Xansys] Re: Volume variation computation

Hi Francesca.

You could try something like this (rough idea):

• Model and mesh the box and a surrounding volume, meaning you have a volume with the box embedded (I think both box and surrounding volume should be solid elements, and they should definitely be sharing nodes).
• The surrounding solid elements should have approx. zero stiffness, so they do not resist the deformation of the box.
• Apply the internal pressure, run the analysis.
• In a copy of the meshed model, use UPGEOM to update the nodes according to the deformed model from the first analysis.
• Measure the volume of only the surrounding solid elements with updated node positions.

If you had to do it with a shell element box (still solid element surrounding), you would need to compensate for a half thickness due to the mid-surface shell.

The accuracy of all this would depend on the deformation of the box. If it is excessive compared to the surrounding solid elements, you may have some problems with convergence, collapsing solid elements etc.

Good luck.

Uffe Dal Eriksen
Ramboll Energy Transition,
Denmark

Classification: Confidential
-----Original Message-----
From: Francesca Pistorio via Xansys <xansys-temp@list.xansys.orgmailto:xansys-temp@list.xansys.org>
Sent: 4. juli 2024 18:09
To: xansys-temp@list.xansys.orgmailto:xansys-temp@list.xansys.org
Cc: Francesca Pistorio <francesca.pistorio@polito.itmailto:francesca.pistorio@polito.it>
Subject: [Xansys] Volume variation computation

Hello everyone,
I hope you can solve my problem. I need to calculate the volume change of a box subjected to pressure on all its internal faces. I have simply created a parallelepiped and modeled it with shell elements. I applied the pressure to all the internal faces of the box and solved it.
Is there a way to calculate the volume change of the box?
Thank you for you help and time.
Best regards,
Francesca
Student at Politecnico di Torino

Xansys mailing list -- xansys-temp@list.xansys.orgmailto:xansys-temp@list.xansys.org To unsubscribe send an email to xansys-temp-leave@list.xansys.orgmailto:xansys-temp-leave@list.xansys.org If you are receiving too many emails from XANSYS please consider changing account settings to Digest mode which will send a single email per day.

Please send administrative requests such as deletion from XANSYS to xansys-mod@tynecomp.co.ukmailto:xansys-mod@tynecomp.co.uk and not to the list _______________________________________________
Xansys mailing list -- xansys-temp@list.xansys.orgmailto:xansys-temp@list.xansys.org To unsubscribe send an email to xansys-temp-leave@list.xansys.orgmailto:xansys-temp-leave@list.xansys.org If you are receiving too many emails from XANSYS please consider changing account settings to Digest mode which will send a single email per day.

Please send administrative requests such as deletion from XANSYS to xansys-mod@tynecomp.co.ukmailto:xansys-mod@tynecomp.co.uk and not to the list

Xansys mailing list -- xansys-temp@list.xansys.orgmailto:xansys-temp@list.xansys.org
To unsubscribe send an email to xansys-temp-leave@list.xansys.orgmailto:xansys-temp-leave@list.xansys.org
If you are receiving too many emails from XANSYS please consider changing account settings to Digest mode which will send a single email per day.

Please send administrative requests such as deletion from XANSYS to xansys-mod@tynecomp.co.ukmailto:xansys-mod@tynecomp.co.uk and not to the list