Learning Forum

[gigihmprayogo]

I am doing reinforced concrete beam column joint analysis using coupled damage-plasticity microplane model. How do i get damage visualisation of homogenized total damage (TOTA), homogenized tension damage (TENS), and homogenized compression damage (COMP) on Workbench

[Wenlong]

Hi, 

The microplane damage output is not directly available in Workbench Mechanical. You would need a command snippet to output that.

"PLESOL, MPDP, TOTA"

Please refer to PLESOL for more information: https://ansyshelp.ansys.com/account/secured?returnurl=/Views/Secured/corp/v192/ans_cmd/Hlp_C_PLESOL.html?q=plesol

And here is an example you can try: 

---

! Graphics power needs to be turned on to view the rebars

/graphics,power

! Enter /post1 module

/post1

! Show result as a png image

/SHOW,png

! Set the frame as the last substep of the 1st step

set,1,last

! Select the SOLID185 elements

esel,s,ename,185

/trlcy,elem,0.5     ! Change them to transparent level 0.5 (0 is solid, 1 is completely transparent)

esel,all

! Set view angle

/view,1,1,1,1

/angle,1,-0.75

! Show the whole section of the reinforcement

/eshape,1

! Plot displacement

plnsol,u,x

! Plot damage

 

plesol, MDPD, TOTA

---

 

Regards,

Wenlong

 

---

Useful Links

---

• How to access Ansys Online Help Document


• How to show full resolution image

 

[gigihmprayogo]

@Wenlong, the solution visualisation shows for displacement only, if i check d snippet, it should be shows 2 image right? displacement and damage..

[Wenlong]

Hmm, what about using these commands:

It works for me:

If it still doesn't work, maybe checking the concrete model? Is it possible you are using the Regularized Elastic Damage Microplane Material model? You can find more info about the material model here: https://ansyshelp.ansys.com/account/secured?returnurl=/Views/Secured/corp/v201/en/ans_mat/microplane.html?q=microplane. You can also do a search "output" in that website to find related information.

 

Regards,

Wenlong

 

---

Useful Links

---

• How to access Ansys Online Help Document


• How to show full resolution image

 

[gigihmprayogo]

I already try your latest snippet but it still wont show..I'm using couple damage-plasticity microplane model, using CPT215 element with 2 extra DOF, here the snippet

Or is there additional step or something that I have to activated?

when I check at solution information it says:

*** WARNING ***                         CP =       0.969   TIME= 15:43:50
 The requested MPDP data is not available.  The PLNSOL command is       
 ignored.

[Wenlong]

Hi,

Apart from your command snippet, I also have the following to assign the material to concrete, and request all the outputs. You can try putting it below your commands and see.

 

Regards,

Wenlong

 

[gigihmprayogo]

Thank you, finally it works, here the visualisation

But another problem comes up , when I change the mesh size..the damage wont show, please advice

[DrDalyO]

Hi gigihmprayogo,

Would you mind posting the full command snippits you used in the end? I am also unable to plot the microplane damages TOTA, TENS, COMP, RW using the PELSOL,MPDP command. Error is "The requested MPDP data is not available."

See the file : Commands

[gigihmprayogo]

@DrDalyo, in prep7 snippet, make sure to request all solution: OUTRES,ALL,ALL

And Here my latest snippet to plot the damage:

/SHOW,PNG

!Change White Background

/RGB,INDEX,100,100,100, 0

/RGB,INDEX, 80, 80, 80,13

/RGB,INDEX, 60, 60, 60,14

/RGB,INDEX, 0, 0, 0,15

 

ESEL,ALL

/VIEW,1,1,1,1

PLNSOL,U,Z

PLNSOL,MPDP,TOTA

PLNSOL,MPDP,COMP

PLNSOL,MPDP,TENS

 

To test my command and make it simple, I'm modeling cube uniaxial test (on my previous post), and assigning the microplane properties on solid body (same format with your attached snippet). But the damage only show if I used single element, if I mesh the cube, the damage plot wont show..still dont know how to figure it out

[gigihmprayogo]

@DrDalyo, if you are still unable to plot the damage, try add command "set,last"  on your post prep command..now i'm able to plot the damage

[vaibhavtaranekar]

ArrayI am unable to view the damage at other steps whenever i try to use Set,2,last or any other substep, i don't get any output.n

[DrDalyO]

Hi vaibhavtaranekar, I found the same issue as you. It seems like the damage outputs do not work in workbench when there is more than 1 step. Could be we have the commands wrong. A workaround that I used was instead of using steps, just use time. So I created a model that goes to 2s, instead of 1s, and then apply the loading conditions differently at 1s and 2s which basically comes out to the same thing as 2 steps. This method then works, and you can output the damage models at different times. I posted a brand new video on this here!:nn

[vaibhavtaranekar]

Looks promising! Thanks for new video!n

[Youssef Abbas]

Hello,

i have this problem. I don't know how to solve it. Can someone help me there?

DISPLAY NODAL SOLUTION,  ITEM=MPDP  COMP=TOTA             

 *** WARNING ***                         CP =       1.641   TIME= 17:51:31
 The requested MPDP data is not available.  The PLNSOL command is       
 ignored.       

[Youssef Abbas]

[Youssef Abbas]

I have the same problem. I don't find a solution.